Structural Engineering Analysi

_________________________________________________________

Structural Engineering Analysis and Design _________________________________________________________

SECOND EDITION ENGR SREEJIT RAGHU MEng DIC ACGI MIStructE CEng MIEM

Ove Arup & Partners International Ltd 13 Fitzroy Street, London W1T 4BQ tel +44 (0) 20 7636 1531 fax +44 (0) 20 7755 2150 email [email protected] internet www.arup.com

Structural Engineering Analysis and Design Second Edition

TABLE OF CONTENTS ACKNOWLEDGEMENTS .....................................................................................................................................13 LIST OF SYMBOLS AND NOTATIONS .............................................................................................................14 1

INTRODUCTION..............................................................................................................................................17

2

CONCEPTS OF COMPUTATIONAL FINITE ELEMENT STRUCTURAL ANALYSIS.......................18

2.1

OVERVIEW OF THE FINITE ELEMENT METHOD ............................................................................................18

2.1.1

GL, ML Static Finite Element Elemental Formulation ...............................................................................................................18

2.1.1.1 The Principle of Virtual Displacements of The Principle of Virtual Work (Equivalent to the Variational Method or The Principle of Minimum Potential Energy) ..................................................................................................................................................................................................................... 18 2.1.1.2 The Method of Weighted Residuals........................................................................................................................................................................ 20

2.1.2 2.1.3 2.1.4 2.1.5

GL, ML Static Finite Element Global Formulation.....................................................................................................................21 GNL, MNL Static Finite Element Elemental Formulation .........................................................................................................24 GNL, MNL Static Finite Element Global Formulation ...............................................................................................................29 How Nonlinear Analysis Varies From Linear Analysis ...............................................................................................................32

2.1.5.1 2.1.5.2 2.1.5.3

Geometric Nonlinearity .......................................................................................................................................................................................... 32 Material Nonlinearity.............................................................................................................................................................................................. 34 Contact and Boundary Conditions Nonlinearity...................................................................................................................................................... 34

2.1.6

GL, ML and GNL, MNL Dynamic Finite Element Elemental and Global Formulation..........................................................34

2.2

STATIC ANALYSIS CONCEPTS .........................................................................................................................35

2.2.1

2.3

Overview of Methods of Structural Static Analyses ....................................................................................................................35

DYNAMIC ANALYSIS CONCEPTS .....................................................................................................................36

2.3.1

Overview of Methods of Structural Dynamic Analyses ...............................................................................................................36

2.3.1.1 2.3.1.2

Modal Analyses ...................................................................................................................................................................................................... 36 Forced Response Analyses...................................................................................................................................................................................... 36

2.3.2

Nature of Trial Solution in Harmonic Frequency Vibrations .....................................................................................................38

2.4 3

STATIC AND DYNAMIC ANALYSES SEQUENCES .............................................................................................39 METHODS OF STATIC ANALYSES.............................................................................................................42

3.1

GL, ML STATIC ANALYSIS BY THE IMPLICIT DIRECT STIFFNESS METHOD ..............................................42

3.1.1 3.1.2 3.1.3 3.1.4

Mathematical Formulation of Analysis.........................................................................................................................................42 Concepts of Geometric Stiffness or P-∆ ∆ (KGA From KEA) Analysis ...........................................................................................43 A A Performing P-∆ ∆ (KG From KE ) Linear Static Analysis – Direct Approach............................................................................48 Performing P-∆ ∆ (KGA From KEA) Linear Static Analysis – Modal Approach; And Hence P-∆ ∆ Based Buckling ...................50

3.1.4.1 3.1.4.2 3.1.4.3 3.1.4.4 3.1.4.5 3.1.4.6 3.1.4.7

Objectives ............................................................................................................................................................................................................... 50 Mathematical Formulation...................................................................................................................................................................................... 50 Critical Load Case Considerations.......................................................................................................................................................................... 52 Modelling (Modal) Imperfections........................................................................................................................................................................... 53 Design..................................................................................................................................................................................................................... 57 Limitations.............................................................................................................................................................................................................. 58 Methodology........................................................................................................................................................................................................... 59

3.1.5

MSC.NASTRAN Decks ..................................................................................................................................................................62

3.1.5.1 3.1.5.2 3.1.5.3

ML, GL Static Analysis .......................................................................................................................................................................................... 62 GL, ML P-∆ (KGA From KEA) Static Analysis......................................................................................................................................................... 71 GL, ML P-∆ (KGA From Exact or Approximate KTA) Static Analysis ..................................................................................................................... 72

3.1.6

Hand Methods Verification............................................................................................................................................................73

3.1.6.1 3.1.6.2 3.1.6.3 3.1.6.4 3.1.6.5 3.1.6.6 3.1.6.7

Static Displacements by the Unit Load Method of the Virtual Work Principle....................................................................................................... 73 BMD and SFD of Structures of Low Static Indeterminacies by Flexibility Analysis.............................................................................................. 76 Bending Moments, Shear Force, and Displacements of Structural Elements by the Stiffness Method ................................................................... 98 Bending Moments and Shear Force of Structures of Low Kinematic Indeterminacies by Moment Distribution .................................................... 99 Summary of Deflections and Effects..................................................................................................................................................................... 123 Member Buckling Check Using The P-∆ Method To Incorporate Imperfections, Residual Stresses .................................................................... 164 Overall Portal Frame and Multi-Storey Building P-∆ Analysis Using The Amplified Sway Method ................................................................... 177

3.2

GL, ML BUCKLING ANALYSIS BY THE IMPLICIT LINEARIZED EIGENVALUE ANALYSIS .........................178

3.2.1

Linearization of Tangent Stiffness Matrix and Formulating The Linear Eigenvalue Problem .............................................178

2


3.2.2 3.2.3 3.2.4

Problem Reduction and Trial Modes in Linear Buckling Analysis ..........................................................................................184 Concepts of Linearized (KGA From KEA) Buckling Analysis.....................................................................................................185 MSC.NASTRAN Decks ................................................................................................................................................................186

3.2.4.1 3.2.4.2

GL, ML (KGA From KEA) Buckling Analysis ........................................................................................................................................................ 186 GL, ML (KGA From Exact or Approximate KTA) Buckling Analysis .................................................................................................................... 192

3.2.5

Hand Methods Verification..........................................................................................................................................................195

3.2.5.1 3.2.5.2

Member or Local (KGA From KEA) Buckling ........................................................................................................................................................ 195 Overall System (KGA From KEA) Buckling............................................................................................................................................................ 203

3.3

GL, MNL PLASTIC COLLAPSE ANALYSIS BY THE IMPLICIT LINEAR SIMPLEX PROGRAMMING ............214

3.3.1 3.3.2 3.3.3 3.3.4

Mathematical Formulation of Analysis.......................................................................................................................................214 Mathematical Proof ......................................................................................................................................................................217 Displacements and Rotations at Collapse ...................................................................................................................................221 Plastic Limit Analysis of Simple Framed Structures .................................................................................................................222

3.3.4.1 3.3.4.2 3.3.4.3

Portal Frame ......................................................................................................................................................................................................... 222 Parabolic Arch ...................................................................................................................................................................................................... 228 Displacements and Rotations at Collapse.............................................................................................................................................................. 229

3.3.5

Plastic Limit Analysis of Rectangular Multi-Storey Multi-Bay Frames with Improved Data Generation ...........................231

3.3.5.1 3.3.5.2 3.3.5.3 3.3.5.4

Two Storey Frame With Concentrated Loading.................................................................................................................................................... 232 Three Storey Frame With Distributed Load .......................................................................................................................................................... 234 Multi-Bay Portal Frame ........................................................................................................................................................................................ 237 Vierendeel Truss ................................................................................................................................................................................................... 239

3.3.6


3.3.6.1 3.3.6.2 3.3.6.3

Plastic Collapse Analysis by Solving Equilibrium Equations ............................................................................................................................... 240 Plastic Collapse Analysis by Virtual Work (Hobbs) ............................................................................................................................................. 244 Plastic Collapse Analysis by Virtual Work (Chryssanthopoulos) ......................................................................................................................... 246

3.4 GNL, MNL, CONTACT NONLINEAR STATIC AND BUCKLING ANALYSIS BY THE IMPLICIT TRACING THE EQUILIBRIUM PATH METHOD ................................................................................................................................262 3.4.1 3.4.2 3.4.3 3.4.4

Mathematical Formulation of Tracing the Equilibrium Path...................................................................................................262 Newton-Raphson Load Control, Displacement Control or Arc-Length Control Algorithm..................................................265 Equilibrium Paths, Stability of Equilibrium Paths, Critical Points, Stability of Critical Points............................................266 MSC.NASTRAN Decks ................................................................................................................................................................269

3.4.4.1 3.4.4.2 3.4.4.3 3.4.4.4 3.4.4.5 3.4.4.6 3.4.4.7

GNL, MNL Load Control, Displacement Control or Arc-Length Control Static Analysis.................................................................................... 269 Nonlinear Static and Linearized Eigenvalue Buckling Analysis ........................................................................................................................... 280 Nonlinear Static and Linear Eigenvalue Modal Dynamic Analysis ...................................................................................................................... 281 Restart From Nonlinear Static Analysis SOL 106 Into Nonlinear Static Analysis SOL 106................................................................................. 282 Restart From Nonlinear Static SOL 106 Into Linear Solution Schemes SOL 107 to SOL 112 ............................................................................. 282 Implicit Nonlinear Static (and Dynamic Analysis) SOL 400 ................................................................................................................................ 282 Implicit Nonlinear Static (and Dynamic Analysis) SOL 600 ................................................................................................................................ 282

3.5

GNL, MNL STATIC AND BUCKLING ANALYSIS BY DYNAMIC RELAXATION.............................................283

3.5.1 3.5.2

4

Dynamic Relaxation of the Explicit Finite Difference Scheme Solving Newton’s Dynamic Equilibrium ODE (LS-DYNA) 283 LS-DYNA (GNL, MNL Explicit Transient) Dynamic Relaxation Cards.................................................................................286

METHODS OF DYNAMIC ANALYSES......................................................................................................288

4.1

GL, ML IMPLICIT REAL MODAL (EIGENVALUE) ANALYSIS ......................................................................288

4.1.1 4.1.2

Mathematical Formulation of Analysis.......................................................................................................................................288 MSC.NASTRAN Decks ................................................................................................................................................................292

4.1.2.1 4.1.2.2 4.1.2.3

GL, ML Real Modal Analysis............................................................................................................................................................................... 292 GL, ML P-∆ (KGA From KEA) Real Modal Analysis ............................................................................................................................................. 293 GL, ML P-∆ (KGA From Exact or Approximate KTA) Real Modal Analysis ......................................................................................................... 295

4.1.3


4.1.3.1 4.1.3.2 4.1.3.3 4.1.3.4 4.1.3.5

Natural Frequency and Free Vibration Response of SDOF Systems..................................................................................................................... 296 Natural Frequencies of MDOF Systems................................................................................................................................................................ 299 Natural Frequencies of Distributed Systems ......................................................................................................................................................... 311 Natural Frequencies By Exactly Solving the Partial Differential Equilibrium Equation ....................................................................................... 312 Approximate Formulae ......................................................................................................................................................................................... 317

4.2

GL, ML IMPLICIT DIRECT COMPLEX MODAL (EIGENVALUE) ANALYSIS ................................................319

4.2.1 4.2.2 4.2.3 4.2.4

Mathematical Formulation of Analysis.......................................................................................................................................319 Complexity of Modes of Vibration ..............................................................................................................................................320 Complex Modal Analysis To Determine Modal Damping Values ............................................................................................320 MSC.NASTRAN Decks ................................................................................................................................................................321

4.2.4.1 4.2.4.2 4.2.4.3

GL, ML Complex Modal Analysis ....................................................................................................................................................................... 321 GL, ML P-∆ (KGA From KEA) Complex Modal Analysis ...................................................................................................................................... 323 GL, ML P-∆ (KGA From Exact or Approximate KTA) Complex Modal Analysis .................................................................................................. 325

4.2.5


3


4.2.5.1 Determination of Damped Natural Frequency and the Maximum Dynamic Displacement, umax for Free Damped Vibration Due to Initial Displacement and/or Initial Velocity by Classically Solving the SDOF Linear ODE and Maximizing the Solution ............................................................. 326

4.3

GL, ML IMPLICIT (REAL) MODAL FREQUENCY RESPONSE ANALYSIS .....................................................329

4.3.1 4.3.2 4.3.3 4.3.4 4.3.5 4.3.6

Nature of the Dynamic Loading Function ..................................................................................................................................329 Mathematical Formulation of Analysis.......................................................................................................................................329 Capability of A Finite Number of Modes To Model The Static and Dynamic Response of Structure...................................334 Complex Response F(ω ω) and Amplification D(ω ω) With Elemental and/or Modal Structural Damping................................337 Representation of A MDOF System As A SDOF system ...........................................................................................................338 MSC.NASTRAN Decks ................................................................................................................................................................340

4.3.6.1 4.3.6.2 4.3.6.3

GL, ML Modal Forced Frequency Response Analysis ......................................................................................................................................... 340 GL, ML P-∆ (KGA From KEA) Modal Forced Frequency Response Analysis ........................................................................................................ 343 GL, ML P-∆ (KGA From Exact or Approximate KTA) Modal Forced Frequency Response Analysis .................................................................... 345

4.3.7


4.3.7.1 Determination of Maximum Dynamic Displacement for Deterministic Frequency Domain Loading by Transforming the Coupled MDOF Linear Damped ODEs To a Set of Independent (Uncoupled) SDOF ODEs and Solving the Independent Equations in a Manner Similar to Solving a SDOF ODE346

4.4

GL, ML IMPLICIT (COMPLEX) MODAL FREQUENCY RESPONSE ANALYSIS .............................................355

4.4.1

4.5

Mathematical Formulation of Analysis.......................................................................................................................................355

GL, ML IMPLICIT DIRECT FREQUENCY RESPONSE ANALYSIS ..................................................................358

4.5.1 4.5.2 4.5.3

Nature of the Dynamic Loading Function ..................................................................................................................................358 Mathematical Formulation of Analysis.......................................................................................................................................358 MSC.NASTRAN Decks ................................................................................................................................................................361

4.5.3.1 4.5.3.2 4.5.3.3

GL, ML Direct Forced Frequency Response Analysis.......................................................................................................................................... 361 GL, ML P-∆ (KGA From KEA) Direct Forced Frequency Response Analysis ........................................................................................................ 371 GL, ML P-∆ (KGA From Exact or Approximate KTA) Direct Forced Frequency Response Analysis..................................................................... 373

4.5.4


4.5.4.1 The Theory of the Dynamic Magnification Factor for Undamped Motion and Hence the Determination of Maximum Dynamic Displacement, umax for Deterministic Harmonic Loading by Classically Solving the SDOF Linear Undamped ODE and Maximizing the Solution........................................... 374 4.5.4.2 The Theory of the Dynamic Magnification Factor for Damped Motion and Hence Determination of Maximum Dynamic Displacement, umax for Deterministic Harmonic Loading by Classically Solving the SDOF Linear Damped ODE and Maximizing the Solution .................................................... 376 4.5.4.3 The Theory of Vibration (Base) Isolation and the Force Transmitted Into Rigid Foundation by the Damped Structure Subjected to Deterministic Harmonic Loading................................................................................................................................................................................................................. 381 4.5.4.4 The Theory of Vibration (Base) Isolation and the Determination of Maximum Dynamic Displacement, umax for Deterministic Harmonic Support Motion (Displacement, Velocity or Acceleration) by Classically Solving the SDOF Linear Damped ODE (in Absolute and Relative Terms) and Maximizing the Solution ........................................................................................................................................................................................................................... 383

4.6 GL, ML FREQUENCY DOMAIN ANALYSIS – DETERMINISTIC AND RANDOM DYNAMIC RESPONSE ANALYSIS .................................................................................................................................................................386 4.6.1 4.6.2

Mathematical Preliminaries of Representing Dynamic Characteristics in the Frequency Domain ......................................386 GL, ML Vibration Testing ...........................................................................................................................................................387

4.6.2.1 4.6.2.2

Vibration Testing for Model Correlation .............................................................................................................................................................. 387 Vibrating Testing For Analysis Procedure Verification ........................................................................................................................................ 390

4.6.3 GL, ML Steady-State Response of Deterministic Periodic (Not Necessarily Harmonic) Long Duration Excitation Utilizing Fourier Series (or Generally Utilizing Fast Fourier Transforms FFT) .................................................................................................391 4.6.3.1 4.6.3.2 4.6.3.3 4.6.3.4 4.6.3.5 4.6.3.6 4.6.3.7 4.6.3.8 4.6.3.9

Fourier Series........................................................................................................................................................................................................ 391 Discrete Fourier Series.......................................................................................................................................................................................... 392 Discrete Fourier Series in Complex Notation........................................................................................................................................................ 393 Double Sided Discrete Fourier Series in Complex Notation ................................................................................................................................. 394 Normalized Double Sided Discrete Fourier Series in Complex Notation.............................................................................................................. 395 Symmetrical Normalized Double Sided Discrete Fourier Series in Complex Notation......................................................................................... 396 Symmetrical Normalized Single Sided Discrete Fourier Series in Complex Notation .......................................................................................... 397 Practicalities of the Specification of the Fast Fourier Transform (FFT) Representation ....................................................................................... 398 MSC.NASTRAN Fast Fourier Transform Analysis Methodology........................................................................................................................ 400

4.6.4 GL, ML Steady-State Response of Random, Gaussian, and Stationary (and Ergodic) Excitations Utilizing Power Spectral Density (PSD) Functions............................................................................................................................................................................403 4.6.4.1 4.6.4.2 4.6.4.3 4.6.4.4 4.6.4.5 4.6.4.6

4.7

Statistic of Time Domain Function ....................................................................................................................................................................... 403 Definition of the Power Spectral Density (PSD)................................................................................................................................................... 407 Validity of the PSD Representation ...................................................................................................................................................................... 410 Generation and Specification of the PSD.............................................................................................................................................................. 411 Statistical Information Provided by the PSD......................................................................................................................................................... 412 MSC.NASTRAN Random Analysis Methodology ............................................................................................................................................... 415

GL, ML IMPLICIT (REAL) MODAL TRANSIENT RESPONSE ANALYSIS ......................................................419

4.7.1 4.7.2 4.7.3 4.7.4 4.7.5 4.7.6

Nature of the Dynamic Loading Function ..................................................................................................................................419 Mathematical Formulation of Analysis.......................................................................................................................................419 Capability of A Finite Number of Modes To Model The Static and Dynamic Response of Structure...................................424 Concepts of Equivalent Static Force ...........................................................................................................................................433 Structural Damping in Time Domain Analyses..........................................................................................................................435 MSC.NASTRAN Decks ................................................................................................................................................................437

4.7.6.1 4.7.6.2

GL, ML Modal Forced Transient Response Analysis ........................................................................................................................................... 437 GL, ML P-∆ (KGA From KEA) Modal Forced Transient Response Analysis.......................................................................................................... 440

4


4.7.6.3

GL, ML P-∆ (KGA From Exact or Approximate KTA) Modal Forced Transient Response Analysis ...................................................................... 442

4.7.7


4.7.7.1 Determination of Maximum Dynamic Displacement for Deterministic Time Domain Loading by Transforming the Coupled MDOF Linear Undamped ODEs To a Set of Independent (Uncoupled) SDOF ODEs and Solving the Independent Equations in a Manner Similar to Solving a SDOF ODE 443 4.7.7.2 Determination of Max Dynamic Displacement for Deterministic Time Domain Support Motion (Displacement, Velocity or Acceleration) by Transforming the Coupled MDOF Linear Undamped ODEs (In Relative Terms) To a Set of Independent (Uncoupled) SDOF ODEs (In Relative Terms) and Solving the Independent Equations in a Manner Similar to Solving a SDOF ODE ............................................................................................................... 452 4.7.7.3 Determination of Maximum Dynamic Displacement for Deterministic Time Domain Loading by Transforming the Coupled Distributed System Linear Damped ODEs (from the governing PDE) To A Set of Independent (Uncoupled) SDOF ODEs and Solving the Independent Equations in a Manner Similar to Solving a SDOF ODE ........................................................................................................................................................................................... 456

4.8

GL, ML IMPLICIT DIRECT TRANSIENT RESPONSE ANALYSIS ...................................................................457

4.8.1 4.8.2 4.8.3

Nature of the Dynamic Loading Function ..................................................................................................................................457 Mathematical Formulation of Analysis.......................................................................................................................................457 MSC.NASTRAN Decks ................................................................................................................................................................460

4.8.3.1 4.8.3.2 4.8.3.3

GL, ML Direct Forced Transient Response Analysis............................................................................................................................................ 460 GL, ML P-∆ (KGA From KEA) Direct Forced Transient Response Analysis .......................................................................................................... 470 GL, ML P-∆ (KGA From Exact or Approximate KTA) Direct Forced Transient Response Analysis ...................................................................... 472

4.8.4


4.8.4.1 Determination of Maximum Dynamic Displacement, umax by Solving the SDOF Undamped/Damped Linear Equation of Motion ODE for Deterministic Time Domain Loading With/Without Initial Conditions Using the Convolution Integral (Duhamel’s integral) ............................................. 473 4.8.4.2 Determination of Maximum Dynamic Displacement, umax by Solving the SDOF Undamped/Damped Linear Equation of Motion ODE (In Relative Terms) for Deterministic Time Domain Support Motion (Displacement, Velocity or Acceleration) With/Without Initial Conditions Using the Convolution Integral (Duhamel’s integral) ............................................................................................................................................................................ 480

4.9

GNL, MNL IMPLICIT AND EXPLICIT DIRECT TRANSIENT RESPONSE ANALYSIS .....................................481

4.9.1 4.9.2 4.9.3 4.9.4 4.9.5

Nature of the Dynamic Loading Function ..................................................................................................................................481 Deterministic Non-Periodic Short Duration Impulse (a.k.a. Blast) Loading Functions With Subsequent Wave Propagation 482 Projectile Crash (a.k.a. Impact) (and Impulsive Blast) Analysis With Subsequent Wave Propagation................................483 Brittle Snap or Redundancy Check Excitation ..........................................................................................................................486 GNL, MNL Explicit Central FD Scheme for Newton’s Dynamic Equilibrium ODE (LS-DYNA).........................................491

4.9.5.1 4.9.5.2 4.9.5.3 4.9.5.4

Solution of Partial or Ordinary Differential Equations Using Finite Difference (FD) Schemes ............................................................................ 491 Mathematical Formulation of Analysis – Explicit Central Finite Difference Scheme........................................................................................... 492 Stability................................................................................................................................................................................................................. 493 Accuracy............................................................................................................................................................................................................... 494

4.9.6

GNL, MNL Implicit Newmark Scheme for Newton’s Dynamic Equilibrium ODE (MSC.NASTRAN)................................495

4.9.6.1 4.9.6.2 4.9.6.3

Mathematical Formulation of Analysis – Implicit Newmark Scheme................................................................................................................... 495 Stability................................................................................................................................................................................................................. 497 Accuracy............................................................................................................................................................................................................... 497

4.9.7 4.9.8

Comparison Between Implicit and Explicit Time Integration Schemes...................................................................................498 MSC.NASTRAN Decks ................................................................................................................................................................500

4.9.8.1 4.9.8.2 4.9.8.3 4.9.8.4 4.9.8.5 4.9.8.6 4.9.8.7

GNL, MNL Direct Forced (Implicit) Transient Response Analysis ...................................................................................................................... 500 Nonlinear Static Analysis and Nonlinear Transient Analysis................................................................................................................................ 504 Restart From Nonlinear Static Analysis SOL 106 Into Nonlinear Transient Analysis SOL 129 ........................................................................... 504 Restart From Nonlinear Transient Analysis SOL 129 Into Nonlinear Transient Analysis SOL 129 ..................................................................... 504 Implicit Nonlinear (Static and) Dynamic Analysis SOL 400 ................................................................................................................................ 505 Implicit Nonlinear (Static and) Dynamic Analysis SOL 600 ................................................................................................................................ 505 Explicit Nonlinear Dynamic Analysis SOL 700 ................................................................................................................................................... 505

4.9.9

LS-DYNA Decks ...........................................................................................................................................................................506

4.9.9.1

GNL, MNL Direct Forced (Explicit) Transient Response Analysis ...................................................................................................................... 506

4.9.10

Hand Methods Verification........................................................................................................................................................508

4.9.10.1 Determination of Displacement Response Time History by Solving the SDOF Nonlinear (in Stiffness, Damping and Displacement) Equation of Motion ODE for Deterministic Time Domain Loading With/Without Initial Conditions by Implicit Newmark-β Time Integration Schemes ..................... 508

5

ADVANCED APPLICATIONS OF METHODS OF STATIC AND DYNAMIC ANALYSES ...............510

5.1

EARTHQUAKE INDUCED VIBRATIONS ..........................................................................................................510

5.1.1 5.1.1.1 5.1.1.2 5.1.1.3 5.1.1.4 5.1.1.5 5.1.1.6 5.1.1.7 5.1.1.8 5.1.1.9 5.1.1.10

Engineering Seismology ...............................................................................................................................................................510 Seismic Risk ......................................................................................................................................................................................................... 510 Physics of the Earth .............................................................................................................................................................................................. 510 Plate Tectonics...................................................................................................................................................................................................... 510 Global Seismicity.................................................................................................................................................................................................. 510 Mechanism of Earthquakes: Elastic Rebound ....................................................................................................................................................... 511 Fault Rupture Classification.................................................................................................................................................................................. 511 Seismic Waves...................................................................................................................................................................................................... 512 Accelerographs and Seismographs........................................................................................................................................................................ 512 Earthquake Location Parameters........................................................................................................................................................................... 513 Estimation of Location of Focus or Epicentre..................................................................................................................................................... 513

5


5.1.1.11 5.1.1.12 5.1.1.13 5.1.1.14 5.1.1.15 5.1.1.16 5.1.1.17 5.1.1.18 5.1.1.19

5.1.2 5.1.2.1 5.1.2.2 5.1.2.3 5.1.2.4 5.1.2.5 5.1.2.6 5.1.2.7 5.1.2.8 5.1.2.9 5.1.2.10 5.1.2.11 5.1.2.12 5.1.2.13 5.1.2.14 5.1.2.15

5.1.3 5.1.3.1 5.1.3.2 5.1.3.3 5.1.3.4 5.1.3.5 5.1.3.6 5.1.3.7 5.1.3.8 5.1.3.9 5.1.3.10 5.1.3.11 5.1.3.12 5.1.3.13

Estimation of Focal Depth .................................................................................................................................................................................. 513 Estimation of Time of Earthquake Occurrence ................................................................................................................................................... 513 Earthquake Magnitude ........................................................................................................................................................................................ 514 Evaluation of Regional Seismicity...................................................................................................................................................................... 516 Intensity .............................................................................................................................................................................................................. 516 Characterisation of Strong Motion...................................................................................................................................................................... 516 Attenuation Relationship..................................................................................................................................................................................... 517 Seismic Hazard Evaluation Procedure: Seismic Hazard Curves and Seismic Hazard Maps ............................................................................... 518 Seismic Hazard Evaluation Procedure: Design Response Spectra ...................................................................................................................... 519

Effect of Local Soil Conditions on the Seismic Hazard..............................................................................................................521 Elastic Soil Properties ........................................................................................................................................................................................... 521 Dynamic Response of Soil .................................................................................................................................................................................... 522 Liquefaction.......................................................................................................................................................................................................... 523 Residual Strength of Liquefied Soils..................................................................................................................................................................... 523 Assessment of Liquefaction Potential ................................................................................................................................................................... 524 Post-Seismic Failure due to Liquefaction.............................................................................................................................................................. 525 Methods of Improving Liquefiable Soils .............................................................................................................................................................. 526 Effect of Soil Layer on Ground Response............................................................................................................................................................. 526 Motion of Shear Waves in Elastic Media.............................................................................................................................................................. 526 Impedance (or Radiation) Effect ......................................................................................................................................................................... 527 Increase in Duration of Strong Motion................................................................................................................................................................ 528 Resonance Effect ................................................................................................................................................................................................ 529 Methods of Evaluating Layer Response.............................................................................................................................................................. 530 Critical Acceleration ........................................................................................................................................................................................... 531 Effect of Local Soil Conditions on Seismic Hazard Design Procedure Summary............................................................................................... 532

Conceptual Structural Design for RC Structures in Seismic Regions .....................................................................................542 Plan Layout........................................................................................................................................................................................................... 542 Elevation............................................................................................................................................................................................................... 542 Beam and Column Axes ....................................................................................................................................................................................... 542 Foundation Design................................................................................................................................................................................................ 543 Columns................................................................................................................................................................................................................ 543 Member Capacity at Connections ......................................................................................................................................................................... 543 Floor Slabs............................................................................................................................................................................................................ 543 Infill Panels........................................................................................................................................................................................................... 543 Building Separation .............................................................................................................................................................................................. 544 Architectural Elements........................................................................................................................................................................................ 544 General Robustness............................................................................................................................................................................................. 544 Detailing Requirements and Ductile Response ................................................................................................................................................... 544 Eurocode 8 Conceptual Design ........................................................................................................................................................................... 544

5.1.4 5.1.5

Methods of Structural Analysis ...................................................................................................................................................547 GL, ML Shock and Response Spectrum Analysis......................................................................................................................548

5.1.5.1 5.1.5.2 5.1.5.3 5.1.5.4 5.1.5.5 5.1.5.6

Nature of the Dynamic Loading Function............................................................................................................................................................. 548 The Response Spectra ........................................................................................................................................................................................... 548 GL, ML SDOF Response Spectrum Analysis – Equivalent Lateral Static Force Method ..................................................................................... 565 GL, ML MDOF Response Spectrum Analysis – Multi-Modal Seismic Analysis ................................................................................................. 570 Example Application EC8 .................................................................................................................................................................................... 576 MSC.NASTRAN Decks ....................................................................................................................................................................................... 585

5.1.6

Reinforced Concrete Design to EC8 for Earthquake Effects Based on Response Spectrum Analysis ..................................590

5.1.6.1 5.1.6.2 5.1.6.3 5.1.6.4 5.1.6.5 5.1.6.6 5.1.6.7 5.1.6.8 5.1.6.9 5.1.6.10

Concepts of Ductility ............................................................................................................................................................................................ 590 Capacity Design for Optimum Location and Sequence of Attainment of Member Capacity ................................................................................ 591 Capacity Design for Favourable Mechanism of Deformation ............................................................................................................................... 591 Introduction of Example Problem ......................................................................................................................................................................... 592 Design Data .......................................................................................................................................................................................................... 592 Beam Design for Vertical Loading According to EC2.......................................................................................................................................... 592 Capacity Check for Seismic Loading of Beams .................................................................................................................................................... 598 Design of Transverse Reinforcement .................................................................................................................................................................... 599 Column Design ..................................................................................................................................................................................................... 600 Detailing of Beams ............................................................................................................................................................................................. 607

5.1.7 Steel Design to EC8 for Earthquake Effects Based on Response Spectrum Analysis .............................................................608 5.1.8 Timber Design to EC8 for Earthquake Effects Based on Response Spectrum Analysis.........................................................609 5.1.9 Masonry Design to EC8 for Earthquake Effects Based on Response Spectrum Analysis ......................................................610 5.1.10 Performance Based Seismic Analysis and Design ....................................................................................................................611 5.2 GL, ML HUMAN FOOTFALL INDUCED VIBRATIONS ..................................................................................612 5.2.1 Limitations ....................................................................................................................................................................................612 5.2.2 Finite Element Mesh and Model Parameters .............................................................................................................................612 5.2.3 (Non-Crowd or Asynchronous) Human Induced Vertical Footfall Vibrations from Walking ..............................................615 5.2.3.1 5.2.3.2 5.2.3.3

Dynamic Response To Vertical Dynamic Forces From Walking on Flat and on Stairs ........................................................................................ 615 Serviceability Acceptance Criteria........................................................................................................................................................................ 626 Practical Solutions ................................................................................................................................................................................................ 628

5.2.4

(Non-Crowd or Asynchronous) Human Induced Vertical Footfall Vibrations from Sports in Halls ...................................629

6


5.2.5 Crowd Induced (Synchronous) Vertical Footfall Vibrations for Gymnasium Floors, Dance Floors, Stadium Tiers, Theatre Tiers and Balconies ...................................................................................................................................................................................630 5.2.6 Crowd Induced (Synchronous) Lateral Vibrations ..................................................................................................................633 5.3 GL, ML DYNAMIC INFLUENCE LINE ANALYSIS FOR TRAIN EXCITATIONS ON BRIDGES.........................636 5.4 GL, ML FLUID (WIND & WATER) - STRUCTURE INTERACTION (AEROELASTIC RESPONSE ANALYSIS) 639 5.4.1 Elementary Hydraulics.................................................................................................................................................................640 5.4.1.1 5.4.1.2

Pipeline Design (Application of the Steady and Unsteady Bernoulli’s Equation)................................................................................................. 640 Elementary Wave Mechanics (Small Amplitude Wave Theory)........................................................................................................................... 725

5.4.2

Static Aeroelastic Response..........................................................................................................................................................732

5.4.2.1 5.4.2.2 5.4.2.3

Along-Flow Direction Drag (Pressure Drag and Skin-Friction Drag) (Limited Amplitude Response) ................................................................. 733 Across-Flow Direction Lift (Pressure Lift and Skin-Friction Lift) (Limited Amplitude Response) ...................................................................... 735 Non-Oscillatory Torsional Divergence (Divergent Amplitude Response) ............................................................................................................ 736

5.4.3

Dynamic Aeroelastic Response ....................................................................................................................................................740

5.4.3.1 Along- and Across-Flow Direction Unsteady Inertial Forces on General Submerged Structures Due to Water Waves (Limited Amplitude Response) 740 5.4.3.2 Along- and Across-Flow Direction Unsteady Inertial Forces on Cylindrical Submerged Structures Due to Water Waves (And Along-Flow Direction Drag Forces Due to Steady Currents) (Limited Amplitude Response)................................................................................................................... 741 5.4.3.3 Along-Flow Direction Gust Response (And Along-Flow Direction Drag Forces Due to Steady Mean Wind) (Limited Amplitude Response) ... 744 5.4.3.4 Along-Flow Direction Buffeting Response (Limited Amplitude Response) ......................................................................................................... 761 5.4.3.5 Across-Flow Direction Von Karman Vortex Shedding Induced Response (Limited Amplitude Response) ......................................................... 762

5.4.4

Dynamic Aeroelastic Stability......................................................................................................................................................777

5.4.4.1 5.4.4.2

Across-Flow Direction Galloping and Stall Flutter (Divergent Amplitude Response).......................................................................................... 777 Across-Flow Direction Classical Flutter (Divergent Amplitude Response) .......................................................................................................... 788

5.5

GL, ML VIBRATION FATIGUE ANALYSIS.....................................................................................................796

5.5.1

Maximum Absolute Principal Stress or Strain Field Generation in the Time or Frequency Domain...................................797

5.5.1.1 5.5.1.2 5.5.1.3 5.5.1.4 5.5.1.5

Choice of Analysis Method................................................................................................................................................................................... 797 GL, ML Pseudo-Static Analysis ........................................................................................................................................................................... 798 GL, ML Transient Analysis .................................................................................................................................................................................. 799 GL, ML Modal Superposition Transient Analysis ................................................................................................................................................ 800 GL, ML Frequency Domain Stationary (and Ergodic) Random Analysis............................................................................................................. 801

5.5.2

Stress-Life (S-N), Strain-Life (E-N) or Crack Propagation LEFM Uniaxial Fatigue Analysis ..............................................802

5.5.2.1 5.5.2.2 5.5.2.3

Stress-Life (S-N) (Total Life) Uniaxial Fatigue Analysis ..................................................................................................................................... 803 Strain-Life (E-N) (Crack Initiation) Uniaxial Fatigue Analysis ............................................................................................................................ 812 Crack Propagation LEFM Uniaxial Fatigue Analysis ........................................................................................................................................... 813

5.5.3

Stress-Life (S-N), Strain-Life (E-N) or Crack Propagation LEFM Multi-axial Fatigue Analysis .........................................814

5.6

GL, ML PASSIVE STRUCTURAL MOTION CONTROL ...................................................................................815

5.6.1

Optimum Stiffness and Mass Distribution..................................................................................................................................815

5.6.1.1 5.6.1.2 5.6.1.3 5.6.1.4 5.6.1.5

Concepts of Forced Frequency Response of Deterministic Periodic Harmonic Load Excitations......................................................................... 815 Concepts of Forced Transient Response of Deterministic Load Excitations ......................................................................................................... 818 Concepts of Forced Frequency Response of Deterministic Periodic Harmonic Base Excitations ......................................................................... 822 Concepts of Forced Transient Response of Deterministic Base Excitations.......................................................................................................... 823 Concepts of Forced Transient Response (Response Spectrum Analysis) of Random Non-Stationary Base Excitations ....................................... 824

5.6.2

Optimum Damping Distribution .................................................................................................................................................825

5.6.2.1 5.6.2.2 5.6.2.3 5.6.2.4

Elemental Damping Mathematical Models ........................................................................................................................................................... 825 Modal Damping Mathematical Models................................................................................................................................................................. 834 Global Damping Mathematical Models ................................................................................................................................................................ 837 Damping Formulation Conclusions ...................................................................................................................................................................... 839

5.6.3

GL, ML Base Isolation Systems...................................................................................................................................................840

5.6.3.1 5.6.3.2 5.6.3.3 5.6.3.4 5.6.3.5

Controlling Displacement Response From Harmonic Load Excitations ............................................................................................................... 840 Controlling Acceleration Response From Harmonic Load Excitations................................................................................................................. 840 Base Isolation - Controlling Displacement Response From Harmonic Base Enforced Motion ............................................................................. 841 Base Isolation - Controlling Acceleration Response From Harmonic Base Enforced Motion .............................................................................. 842 Base Isolation – Controlling Force Transmitted Into Foundation From Harmonic Load Excitations.................................................................... 844

5.6.4

GL, ML Tuned Mass Damper (TMD) Systems ..........................................................................................................................845

5.6.4.1 5.6.4.2 5.6.4.3 5.6.4.4 5.6.4.5 5.6.4.6

Damped SDOF System Subject to Harmonic Force and Support Motion Excitations .......................................................................................... 848 Undamped Structure, Undamped TMD System Subject to Harmonic Force Excitation ....................................................................................... 849 Undamped Structure, Damped TMD System Subject to Harmonic Force Excitation ........................................................................................... 851 Undamped Structure, Damped TMD System Subject to Harmonic Support Motion ............................................................................................ 857 Damped Structure, Damped TMD System Subject to Harmonic Force and Support Motion................................................................................ 859 TMD Analysis Summary (Warburton, 1982)........................................................................................................................................................ 861

5.6.5

GL, ML Tuned Slosh Damper (TSD) Systems ..........................................................................................................................863

5.6.5.1 5.6.5.2 5.6.5.3 5.6.5.4 5.6.5.5 5.6.5.6

When To Employ TSDs........................................................................................................................................................................................ 863 Operations of TSDs .............................................................................................................................................................................................. 863 Deep or Shallow Tank?......................................................................................................................................................................................... 871 Testing .................................................................................................................................................................................................................. 872 Miscellaneous Design Information ....................................................................................................................................................................... 873 Design Procedure for Deep Tank TSDs ................................................................................................................................................................ 874

5.7 5.8

GL, ML ACTIVE STRUCTURAL MOTION CONTROL – CONTROL SYSTEM ANALYSIS...............................875 FIBRE REINFORCED POLYMER (FRP) ANALYSIS AND DESIGN ..................................................................876

7


5.8.1 5.8.2 5.8.3 5.8.4 5.8.5 5.8.6

Introduction ..................................................................................................................................................................................876 The Reinforcement Fibre .............................................................................................................................................................876 The Polymer (Resin) Matrix ........................................................................................................................................................878 The Additives ................................................................................................................................................................................880 The Composite Laminate Forming Processes.............................................................................................................................881 Modelling and Analyzing Fibre Reinforced Polymer (FRP) Composite Laminates in MSC.NASTRAN .............................882

5.8.6.1 5.8.6.2 5.8.6.3 5.8.6.4

The Ply.................................................................................................................................................................................................................. 882 The Composite Laminate, Sandwich Structures and Structural Members with Attached Laminates .................................................................... 886 Failure Mode and Failure Criteria of the Composite Laminate ............................................................................................................................. 888 MSC.NASTRAN Finite Element Modelling of Composite Laminate Summary .................................................................................................. 890

6 FINITE ELEMENT MODELLING TECHNIQUES AND MSC.NASTRAN CARDS COMMON TO ALL ANALYSES....................................................................................................................................................892 6.1 6.2 6.3

INPUT DECK .DAT FORMAT ...........................................................................................................................892 GRID CARDS ...................................................................................................................................................895 FINITE ELEMENT MODELLING TECHNIQUES ..............................................................................................896

6.3.1 Nature of the Finite Element Method..........................................................................................................................................896 6.3.2 Finite Element Displacement Interpolation Function, Output Stress Variation, and Corresponding Order of Error in Displacement and Stress............................................................................................................................................................................897 6.3.2.1 6.3.2.2 6.3.2.3 6.3.2.4

One Dimensional Beam Finite Element ................................................................................................................................................................ 898 Two Dimensional Shell Elements (In-Plane Plane Stress or Plane Strain Membrane Stiffness) ........................................................................... 900 Two Dimensional Shell Elements (Out of Plane Bending, Shear and Torsional Plate Stiffness) ......................................................................... 903 Three Dimensional Solid Elements....................................................................................................................................................................... 907

6.3.3

Finite Element Modelling For Static Analyses ...........................................................................................................................908

6.3.3.1 6.3.3.2

Choice of Finite Element to Model the Load Path and Deformation..................................................................................................................... 908 Concepts of Stiffness ............................................................................................................................................................................................ 908

6.3.4

Finite Element Modelling For Dynamic Analyses......................................................................................................................909

6.3.4.1 6.3.4.2

Mass and Stiffness Distribution ............................................................................................................................................................................ 909 Nonstructural Mass ............................................................................................................................................................................................... 909

6.3.5 Modelling Mechanisms With Inertia Relief – Modelling Displacement Effects Due to Applied Loads On Systems in Conditionally Stable Equilibrium.............................................................................................................................................................911 6.3.6 Submodelling Techniques for Static Analysis ............................................................................................................................913 6.3.6.1 6.3.6.2 6.3.6.3 6.3.6.4 6.3.6.5 6.3.6.6

Submodelling by Substructuring – Static Condensation (Guyan Reduction) using Superelements....................................................................... 913 Submodelling – Boundary Internal Force Method ................................................................................................................................................ 919 Submodelling – Boundary Internal Force Method of Substructure Isostatically Mounted Over Rest of Structure................................................ 922 Boundary Enforced Displacement Method ........................................................................................................................................................... 923 Numerical Example of Submodelling ................................................................................................................................................................... 924 Static Submodelling Methods Summary ............................................................................................................................................................... 929

6.3.7

Submodelling Techniques for Dynamic Analysis .......................................................................................................................930

6.3.7.1 6.3.7.2 6.3.7.3

Submodelling by Substructuring - Static Condensation (Guyan Reduction) using Superelements ....................................................................... 930 Submodelling by Substructuring - Generalized Dynamic Reduction (GDR) using Superelements....................................................................... 930 Submodelling by Substructuring - Component Mode Synthesis (CMS) using Superelements.............................................................................. 930

6.3.8 Modelling Flat Plates Using 2D Shells or 1D Grillages..............................................................................................................931 6.3.9 Modelling Down-Stand Beams on Structural Floors, Pile Caps and Changes in Thickness of Plates ...................................931 6.3.10 Modelling Stiffened Plates..........................................................................................................................................................931 6.3.11 Modelling Connections ...............................................................................................................................................................932 6.3.12 Modelling Spot Welds.................................................................................................................................................................933 6.3.13 Modelling Bolts ...........................................................................................................................................................................933 6.3.14 Modelling Applied Loads ...........................................................................................................................................................934 6.3.14.1 6.3.14.2 6.3.14.3

Applied Concentrated Loads on One Dimensional Elements.............................................................................................................................. 934 Applied Face and Line Loads on Two and Three Dimensional Elements ........................................................................................................... 934 Applied Concentrated Loads on Two and Three Dimensional Elements ............................................................................................................ 935

6.3.15 6.3.16 6.3.17 6.3.18 6.3.19

Modelling Support Conditions...................................................................................................................................................936 Primary and Secondary Component in Dynamic Analysis .....................................................................................................937 Modelling Rigid Body Motion....................................................................................................................................................937 Meshing Strategies......................................................................................................................................................................938 Mesh Transition Techniques......................................................................................................................................................939

6.3.19.1 6.3.19.2 6.3.19.3 6.3.19.4

Connecting 1D Elements to 2D Elements ........................................................................................................................................................... 939 Connecting 2D Elements to 3D Elements ........................................................................................................................................................... 940 Connecting 1D Elements to 3D Elements ........................................................................................................................................................... 942 Fine to Coarse Mesh Transitions in Shell Meshes............................................................................................................................................... 942

6.3.20 Stress Singularity (Artificial Stress Concentration) and St. Venant’s Principle in Linear and Nonlinear (Material) Analysis 943 6.3.21 Modelling Preload (Prestress)....................................................................................................................................................945 6.3.21.1

Temperature Load Method.................................................................................................................................................................................. 945

8


6.3.21.2 6.3.21.3

MPC Constraint Method ..................................................................................................................................................................................... 945 GAP Element Method......................................................................................................................................................................................... 945

6.3.22 6.3.23 6.3.24

Modelling Symmetry ..................................................................................................................................................................946 Multi-Point Constraints (MPC) ................................................................................................................................................947 Model Checkout ..........................................................................................................................................................................949

6.3.24.1 Grid Point Singularities (AUTOSPC, EPZERO, K6ROT, SNORM).................................................................................................................. 949 6.3.24.2 Mechanism Singularity of Stiffness Matrix (MAXRATIO, BAILOUT)............................................................................................................. 952 6.3.24.3 Grid Point Singularities (AUTOSPC, K6ROT) and Local and Global Mechanism Singularity (MAXRATIO, BAILOUT) for Linear, Nonlinear, Static and Dynamic Solutions................................................................................................................................................................................................ 954 6.3.24.4 Ill-Conditioning of Stiffness Matrix (EPSILON, Load and Reaction Discrepancy PRTRESLT)........................................................................ 955 6.3.24.5 Grid Point Weight Generator .............................................................................................................................................................................. 957 6.3.24.6 Displacement Compatibility Check .................................................................................................................................................................... 957 6.3.24.7 Element Quality Checks ..................................................................................................................................................................................... 958 6.3.24.8 Maximum Values................................................................................................................................................................................................ 959 6.3.24.9 Element Orientation Check................................................................................................................................................................................. 959 6.3.24.10 Duplicate Grid and Element Check................................................................................................................................................................... 959 6.3.24.11 Element Summary Table................................................................................................................................................................................... 959 6.3.24.12 Unconstrained Equilibrium Check (Grounding Check) .................................................................................................................................... 960 6.3.24.13 Deformed Shape ............................................................................................................................................................................................... 962 6.3.24.14 Massless Mechanisms....................................................................................................................................................................................... 962

6.3.25 6.3.26

Isoparametric Elements and Numerical Integration ..............................................................................................................963 Element and Nodal Stress Recovery .........................................................................................................................................970

6.3.26.1 6.3.26.2 6.3.26.3 6.3.26.4 6.3.26.5

Stress Recovery at Gauss Points ......................................................................................................................................................................... 970 Extrapolation of Stress From Gauss Points to Element Grids ............................................................................................................................. 971 (Transformation into Global Coordinates and) Averaging of the Elemental Grid Stresses to Yield the Grid Point Stresses............................... 972 Element Stress Recovery Procedures in MSC.NASTRAN ................................................................................................................................. 973 Grid Point Stresses in MSC.NASTRAN ............................................................................................................................................................. 977

6.3.27 6.3.28

Full Integration Quadrature, Reduced Integration Quadrature and Optimal Gauss Sampling Points ..............................979 Stress Interpretation...................................................................................................................................................................981

6.3.28.1 6.3.28.2 6.3.28.3

State of Stress i.e. Global Coordinate Stress Tensors σxx , σyy , σzz , τxy , τyz , τzx ................................................................................................. 982 Failure Criteria.................................................................................................................................................................................................... 983 Deriving Forces (Moments, Shear, Torsion & Axial Force) from Stresses in Shells........................................................................................... 990

6.3.29 6.3.30

The Element Strain Energy Density..........................................................................................................................................991 Error Estimation.........................................................................................................................................................................993

6.3.30.1 GL, ML Analysis Error Estimation: h- or p- Refinement.................................................................................................................................... 993 6.3.30.2 GNL, MNL Analysis Error Estimation: h- or p- Refinement .............................................................................................................................. 993 6.3.30.3 Adaptive Analysis in MSC.NASTRAN with p-Elements ................................................................................................................................... 994 6.3.30.4 Stress Discontinuity Error Estimator................................................................................................................................................................... 997 6.3.30.5 Hand Verification: Deriving Stresses From Forces (Axial, Moments, Shear and Torsion) in Beam Elements and Stresses Due to External Loading of General Shell and Solid Continuum .................................................................................................................................................................. 1000

6.4

STIFFNESS ELEMENT CARDS .......................................................................................................................1003

6.4.1 6.4.2

Scalar CELAS Element ..............................................................................................................................................................1004 One-Dimensional Element Cards ..............................................................................................................................................1005

6.4.2.1 6.4.2.2 6.4.2.3 6.4.2.4

Axial and Torsional Stiffness CROD, CONROD, CTUBE Elements ................................................................................................................. 1005 CBAR Element ................................................................................................................................................................................................... 1008 CBEAM Element................................................................................................................................................................................................ 1018 CBEND Element ................................................................................................................................................................................................ 1019

6.4.3

Two-Dimensional Element Cards..............................................................................................................................................1020

6.4.3.1 6.4.3.2 6.4.3.3

Transverse Bending, Transverse Shear and In-Plane Membrane (Plane Stress or Plane Strain) CQUAD4, CQUAD8, CTRIA3, CTRIA6 Elements 1020 In-Plane Shear and Extension CSHEAR Elements ............................................................................................................................................. 1023 CRACK2D.......................................................................................................................................................................................................... 1023

6.4.4

Three-Dimensional Element Cards ...........................................................................................................................................1024

6.4.4.1 6.4.4.2 6.4.4.3 6.4.4.4

CHEXA8 or CHEXA20 Element........................................................................................................................................................................ 1025 CPENTA6 or CPENTA15 Element .................................................................................................................................................................... 1025 CTETRA4 or CTETRA10 Element .................................................................................................................................................................... 1025 CRACK3D.......................................................................................................................................................................................................... 1025

6.5 6.6

MASS ELEMENT CARDS ...............................................................................................................................1026 DAMPING ELEMENT CARDS ........................................................................................................................1028

6.6.1 6.6.2

Viscous Damping Elements CDAMP and CVISC....................................................................................................................1028 Structural Damping Elements ...................................................................................................................................................1028 6.7 GENERAL NONLINEAR EXCITATION FREQUENCY DEPENDENT SPRING AND LINEAR EXCITATION FREQUENCY DEPENDENT DAMPER CBUSH (PBUSH AND PBUSHT) ELEMENT ............................................1029 6.8 ONE DIMENSIONAL NONLINEAR SPRING AND NONLINEAR DAMPER CBUSH1D (PBUSH1D) ELEMENT

6.9

1030 MATERIAL CARDS........................................................................................................................................1031

6.9.1 6.9.2

Linear, Elastic, Isotropic Material Card for 1-D, 2-D and 3-D Elements MAT1 ..................................................................1031 Linear, Elastic, Anisotropic Elastic Material for Shell MAT2 and Solid Elements MAT9 ..................................................1031

9


6.9.3

6.10 6.11 6.11.1

6.12

Single Point Constraints (SPCs) ..............................................................................................................................................1035

LINEAR OPTIMIZATION SOL 200 .............................................................................................................1036

6.12.1 6.12.2 6.12.3

6.13 7

Linear, Elastic, Orthotropic Elastic Material for Shell Elements MAT8 and Solid Elements MAT9 .................................1031

RIGID ELEMENT CARDS ............................................................................................................................1032 BOUNDARY CONDITIONS ...........................................................................................................................1035 Objective Function and Constraints........................................................................................................................................1036 Design Variables and Constraints ...........................................................................................................................................1036 Optimization Control Parameters ...........................................................................................................................................1037 COMPUTATIONAL MEMORY AND PROCESSING POWER DEMAND..........................................................1037

LS-DYNA CARDS .........................................................................................................................................1038

7.1 7.2

KEYWORD FORMAT OF INPUT DECK .........................................................................................................1038 OUTPUT CARDS ............................................................................................................................................1038

7.2.1 7.2.2

ASCII Output Files.....................................................................................................................................................................1038 BINARY Output Files ................................................................................................................................................................1039 7.3 NODE CARDS ................................................................................................................................................1040 7.4 STIFFNESS ELEMENT CARDS .......................................................................................................................1040 7.4.1 Spring Element Cards ................................................................................................................................................................1042 7.4.2 Beam Element Cards ..................................................................................................................................................................1043 7.4.3 Shell (QUAD4, QUAD8, TRIA3, TRIA6) Element Cards.......................................................................................................1044 7.4.4 Solid (Brick, Wedge, Tetrahedral) Element Cards ..................................................................................................................1046 7.5 MASS AND INERTIA ELEMENT CARDS ........................................................................................................1049 7.6 DAMPING CARDS ..........................................................................................................................................1050 7.7 RIGID ELEMENT CARDS AND STRUCTURAL INTERNAL CONSTRAINTS ...................................................1051 7.7.1 Rigid Body ...................................................................................................................................................................................1051 7.7.1.1 7.7.1.2 7.7.1.3 7.7.1.4 7.7.1.5

Formulation of Rigid Body Joint ........................................................................................................................................................................ 1051 Rigid Body With Mass And Inertia Properties From A Set Of Nodes ................................................................................................................ 1051 Rigid Body With Mass And Inertia Properties From An Element ...................................................................................................................... 1051 Extra Nodes on Rigid Bodies.............................................................................................................................................................................. 1052 Merging Rigid Bodies......................................................................................................................................................................................... 1052

7.7.2 7.7.3

Rigidwall......................................................................................................................................................................................1052 Constraints Between DOFs ........................................................................................................................................................1053

7.7.3.1

Interpolation Constraint ...................................................................................................................................................................................... 1053

7.7.4 7.7.5

Global Restraints ........................................................................................................................................................................1053 Welds and Rivets.........................................................................................................................................................................1054

7.7.5.1 7.7.5.2 7.7.5.3 7.7.5.4 7.7.5.5 7.7.5.6 7.7.5.7

Generalized Spot Weld ....................................................................................................................................................................................... 1054 Generalized Fillet Weld ...................................................................................................................................................................................... 1054 Generalized Butt Weld........................................................................................................................................................................................ 1054 Generalized Cross-Fillet Weld ............................................................................................................................................................................ 1054 Generalized Combined Weld .............................................................................................................................................................................. 1054 Mass-Less Spotweld ........................................................................................................................................................................................... 1054 Mass-Less Rivet.................................................................................................................................................................................................. 1054

7.7.6

Concrete Rebars..........................................................................................................................................................................1054

7.8

BOUNDARY CONDITIONS CARDS ................................................................................................................1055

7.8.1 7.8.2 7.8.3

Single Point Constraints SPCs ...................................................................................................................................................1055 Non-Reflecting Boundaries ........................................................................................................................................................1055 Contact Cards .............................................................................................................................................................................1056

7.8.3.1 7.8.3.2 7.8.3.3 7.8.3.4 7.8.3.5 7.8.3.6

Rigidwall Contact ............................................................................................................................................................................................... 1056 Surface To Surface Contact ................................................................................................................................................................................ 1056 Single Surface Contact........................................................................................................................................................................................ 1056 Nodes to Surface Contact.................................................................................................................................................................................... 1056 Eroding Contacts ................................................................................................................................................................................................ 1056 Tied Interface...................................................................................................................................................................................................... 1056

7.9 8

RESTART CAPABILITIES ..............................................................................................................................1057 STRUCTURAL ENGINEERING ................................................................................................................1058

8.1

CONCEPTUAL STRUCTURAL DESIGN ..........................................................................................................1058

8.1.1 8.1.2

Spans and Span to Depth Ratios................................................................................................................................................1058 Steel Single-Storey Buildings .....................................................................................................................................................1059

10


8.1.2.1 8.1.2.2 8.1.2.3

Universal Beam – Universal Column (No Pinned or Two-Pinned) Portal Frame ............................................................................................... 1059 Universal Beam – Universal Column (Three-Pinned) Portal Frame ................................................................................................................... 1062 Truss – Stanchion Portal Frame .......................................................................................................................................................................... 1063

8.1.3

Steel and Reinforced Concrete Multi-Storey (Potentially Tall) Buildings .............................................................................1067

8.1.3.1 8.1.3.2 8.1.3.3 8.1.3.4 8.1.3.5 8.1.3.6 8.1.3.7

Building Geometry and Anatomy ....................................................................................................................................................................... 1067 Vertical Gravity and Lateral Stability Systems ................................................................................................................................................... 1070 In-Plane Stability (Diaphragm Action) ............................................................................................................................................................... 1082 Torsional Stability System .................................................................................................................................................................................. 1085 Movement Joints................................................................................................................................................................................................. 1086 Transfer Structures.............................................................................................................................................................................................. 1087 Structural Floor Systems..................................................................................................................................................................................... 1099

8.1.4

Steel, Reinforced Concrete and Masonry Bridges....................................................................................................................1100

8.1.4.1 8.1.4.2 8.1.4.3 8.1.4.4 8.1.4.5 8.1.4.6 8.1.4.7

Steel and Reinforced Concrete Prismatic (Box or Plate) Girder Bridge.............................................................................................................. 1101 Steel and Reinforced Concrete Haunched (Box or Plate) Girder Bridge............................................................................................................. 1102 Steel Truss Bridge............................................................................................................................................................................................... 1103 Steel Portal Bridge .............................................................................................................................................................................................. 1107 Steel, Reinforced Concrete or Masonry Arch Bridge.......................................................................................................................................... 1108 Steel Cable Stayed Bridge................................................................................................................................................................................... 1109 Steel Suspension Bridge ..................................................................................................................................................................................... 1110

8.1.5 8.1.6 8.1.7 8.1.8 8.1.9

Steel Towers ................................................................................................................................................................................1112 Steel Masts...................................................................................................................................................................................1113 Steel Space Roofs ........................................................................................................................................................................1114 Steel Cable Roofs ........................................................................................................................................................................1115 Steel Grandstands .......................................................................................................................................................................1116

8.1.9.1 8.1.9.2 8.1.9.3

Cantilever Grandstand ........................................................................................................................................................................................ 1116 Front Girder Grandstand ..................................................................................................................................................................................... 1116 Cable Suspended Grandstand.............................................................................................................................................................................. 1116

8.1.10 8.1.11

Reinforced Concrete Shell Roofs .............................................................................................................................................1117 Timber Single-Storey Buildings...............................................................................................................................................1118

8.1.11.1 8.1.11.2 8.1.11.3

Beam – Column (No Pinned or Two-Pinned) Portal Frame.............................................................................................................................. 1118 Beam – Column (Three-Pinned) Portal Frame.................................................................................................................................................. 1119 Truss – Stanchion Portal Frame ........................................................................................................................................................................ 1120

8.1.12

Timber Multi-Storey Buildings................................................................................................................................................1139

8.1.12.1

Timber Floors ................................................................................................................................................................................................... 1139

8.1.13

Masonry Single- and Multi-Storey Buildings .........................................................................................................................1140

8.1.13.1

Lateral Stability Systems .................................................................................................................................................................................. 1140

8.2

APPRECIATION OF LOADING, ULS AND SLS LOAD CASES .......................................................................1141

8.2.1 8.2.2 8.2.3

Load Cases...................................................................................................................................................................................1141 Load Factors ...............................................................................................................................................................................1147 Load Combinations ....................................................................................................................................................................1148 8.3 STANDARD CONSTRUCTION MATERIAL PROPERTIES ...............................................................................1150 8.3.1 Steel, Aluminium and Concrete.................................................................................................................................................1150 8.3.2 Stainless Steel ..............................................................................................................................................................................1152 8.3.3 Cast Iron......................................................................................................................................................................................1156 8.3.4 Wrought Iron ..............................................................................................................................................................................1157 8.4 REINFORCED CONCRETE DESIGN TO BS 8110-PART 1:1997 (BUILDINGS) AND BS 5400-PART 4 (BRIDGES)

1159 8.4.1

ULS Rectangular Beam Design – Bending, Shear and Torsion Effects .................................................................................1159

8.4.1.1 8.4.1.2

Bending Effects .................................................................................................................................................................................................. 1159 Shear and Torsion Effects ................................................................................................................................................................................... 1164

8.4.2 8.4.3 8.4.4

Concepts of Moment Redistribution .........................................................................................................................................1167 ULS Structural Floor Design – Reinforced Concrete ..............................................................................................................1176 ULS Structural Floor Design – Prestressed Concrete..............................................................................................................1177

8.4.4.1 8.4.4.2

(Precast) Pre-Tensioned ...................................................................................................................................................................................... 1177 (Cast Insitu) Post-Tensioned Concrete Floor Systems ........................................................................................................................................ 1177

8.4.5 8.4.6 8.4.7 8.4.8 8.4.9 8.4.10 8.4.11

ULS Column Design – Bending, Axial, Shear and Torsion Effects ........................................................................................1178 ULS Wall Design.........................................................................................................................................................................1179 ULS Connection Design..............................................................................................................................................................1180 ULS Fire Protection Design .......................................................................................................................................................1181 SLS Durability Design ................................................................................................................................................................1182 SLS Deflection Computation and Criteria..............................................................................................................................1183 SLS Crack Width Calculations................................................................................................................................................1193 8.5 PRESTRESSED CONCRETE ANALYSIS AND DESIGN ....................................................................................1194 8.6 STEEL DESIGN TO BS 5950-PART 1:2000 (BUILDINGS) .............................................................................1244 8.6.1 ULS Beam and Column Design – Bending (Incorporating High Shear Effects), Axial, Shear and Buckling Effects ........1244 8.6.2 ULS Plate Girder Beam and Column Design – Bending (Incorporating High Shear Effects), Axial, Shear and Buckling Effects 1246

11


8.6.3

ULS Structural Floor Design – Composite Steel and Reinforced Concrete...........................................................................1247

8.6.3.1 Floor Framing ..................................................................................................................................................................................................... 1247 8.6.3.2 Simple Steel I-Beam With Non-Composite or Composite Precast (Hollow) Slabs ............................................................................................. 1248 8.6.3.3 Prismatic Steel I-Beam Encased in T-section Reinforced Concrete, Flat Part of the T- Above the Top Flange of I-Beam................................. 1248 8.6.3.4 Prismatic Steel I-Beam Shear Studded Into Flat-Soffit Reinforced Concrete Slab.............................................................................................. 1248 8.6.3.5 Prismatic Steel I-Beam Shear Studded Into (Parallel Or Perpendicular Ribbed) Metal Deck With Reinforced Concrete................................... 1249 8.6.3.6 Prismatic Steel Plate Girder Shear Studded into Flat-Soffit Reinforced Concrete or (Parallel or Perpendicular Ribbed) Metal Deck with Reinforced Concrete............................................................................................................................................................................................................ 1250 8.6.3.7 Prismatic Steel I-Beam With Stub Girder And Reinforced Concrete Slab .......................................................................................................... 1250 8.6.3.8 Prismatic Steel I-Beam With Web Openings, Castellated Beam, Cellular Beam or Westok Beam Shear Studded into Flat-Soffit Reinforced Concrete or (Parallel or Perpendicular Ribbed) Metal Deck with Reinforced Concrete ...................................................................................................... 1251 8.6.3.9 Prismatic Steel Warren (or Modified Warren) Truss or Pratt Truss, Both With or Without a Vierendeel Panel in the Middle (for the Main Mechanical Duct) Shear Studded into Flat-Soffit Reinforced Concrete or (Parallel or Perpendicular Ribbed) Metal Deck with Reinforced Concrete....... 1258 8.6.3.10 Nonprismatic Tapered (Shallower at the Supports) Steel Plate Girder Shear Studded Into (Parallel or Perpendicular Ribbed) Metal Deck with Reinforced Concrete............................................................................................................................................................................................................ 1258

8.6.4 8.6.5 8.6.6 8.6.7 8.6.8 8.6.9 8.6.10 8.6.11 8.6.12

ULS Composite Column Design ................................................................................................................................................1259 ULS Connection Design..............................................................................................................................................................1260 ULS Bearing and Joints Design .................................................................................................................................................1261 ULS Brittle Fracture Design ......................................................................................................................................................1262 ULS Fatigue Design ....................................................................................................................................................................1262 ULS Fire Protection Design .......................................................................................................................................................1263 SLS Human Induced Vibration ...............................................................................................................................................1265 SLS Deflection Criteria ............................................................................................................................................................1266 SLS Corrosion Protection ........................................................................................................................................................1268 8.7 STEEL DESIGN TO BS 5400-PART 3 (BRIDGES)..........................................................................................1270 8.8 TIMBER DESIGN TO EC5 .............................................................................................................................1271 8.8.1 ULS Beam and Column Design .................................................................................................................................................1273 8.8.2 ULS Dowel (Nailed, Screwed, Bolted, Doweled) Connection Design......................................................................................1274 8.8.3 ULS Fire Protection Design .......................................................................................................................................................1275 8.9 MASONRY DESIGN TO BS 5628 ...................................................................................................................1276

9

GEOTECHNICAL ENGINEERING...........................................................................................................1277

9.1 9.2 9.3 9.4

BASIC SOIL MECHANICS .............................................................................................................................1277 SLOPE STABILITY ANALYSIS .......................................................................................................................1284 EARTH PRESSURE ANALYSIS AND RETAINING WALL DESIGN .................................................................1288 FOUNDATION DESIGN ..................................................................................................................................1312

9.4.1 9.4.2 9.4.3 9.4.4 9.4.5 9.4.6 9.4.7

9.5

Scheme Design.............................................................................................................................................................................1312 Allowable Bearing Pressure .......................................................................................................................................................1316 Pad Footing .................................................................................................................................................................................1318 Strip Footing ...............................................................................................................................................................................1329 Raft Foundation ..........................................................................................................................................................................1330 Basement Foundation .................................................................................................................................................................1331 Piled Foundation.........................................................................................................................................................................1336 SETTLEMENT ANALYSIS ..............................................................................................................................1341

10

CONVERSION FACTORS.........................................................................................................................1348

BIBLIOGRAPHY.................................................................................................................................................1349

12


ACKNOWLEDGEMENTS My humble gratitude to the Almighty, to Whom this and all work is dedicated. A special thank you also to my teachers at Imperial College of Science, Technology and Medicine, London and my fellow engineering colleagues at Ove Arup and Partners London and Ramboll Whitbybird London.

Engr Sreejit Raghu

13


LIST OF SYMBOLS AND NOTATIONS Elemental Notations {y} [N] {f} {d} {b} [k] [m] [c] {p} [T] W

= = = = = = = = = = =

displacement function shape functions matrix element forces in element axes including fixed end forces element deformation in element axes element body forces element constitutive matrix element mass matrix element viscous damping matrix element nodal loading vector transformation matrix work done by external loads

SDOF, MDOF and Modal Dynamic Equation of Motion Notations m = [M] = c = [C] = k = [K] = u = {u},{U}= {P} = Mi, [M] = Ci, [C] = Ki, [K] = ξi, {ξi} =

SDOF mass Global MDOF mass matrix SDOF viscous damping constant Global MDOF viscous damping matrix SDOF stiffness Global MDOF stiffness matrix SDOF displacement Global MDOF displacement matrix Global nodal loading vector Modal (generalized) mass and modal (generalized) mass matrix Modal (generalized) damping and modal (generalized) damping matrix Modal (generalized) stiffness and modal (generalized) stiffness matrix Modal displacement response and modal displacement response vector

SDOF Dynamic Notations ωn ωd ω

c ccr ζ δ

= = = = = = =

Natural circular frequency, (k/m)1/2 Damped natural circular frequency, ωn(1−ζ2)1/2 Frequency of forcing function Viscous damping constant Critical viscous damping constant, 2(km)1/2 = 2mωn Damping ratio (fraction of critical), c/ccr Logarithmic decrement

SDOF Free Vibrational Notations G

=

Complex starting transient response function, G = GR + iGI

SDOF Time Domain Loading and Transient and Steady-State Response Notations P(t) p0 p0/k D(t)

= = = =

Loading function Force excitation amplitude Static displacement Dynamic amplification factor

14


Dmax u(t) umax

= = =

Maximum dynamic amplification factor Displacement response, D(t)(p0/k) Maximum displacement response, Dmax(p0/k)

Modal Time Domain Loading and Transient and Steady-State Notations {P(t)} Pi(t) p0i p0i/Ki Di (t) Di max ξi(t) ξi max {u(t)}

= = = = = = = = =

Loading function vector Modal loading function, Pi(t) = {φi}T {P(t)} Modal force excitation amplitude Modal static displacement Modal dynamic amplification factor Modal maximum dynamic amplification factor Modal displacement response, ξi(t) = Di(t)p0i/Ki Modal maximum displacement response, ξi max = Di max p0i/Ki Displacement response vector, {u(t)} = [Φ]{ξ(t)}

SDOF Frequency Domain Loading and Steady-State Response Notations P(t) P(ω) p0 p0/k D(ω) Dresonant Dmax F(ω) H(ω) Fresonant Fmax u(t) uresonant umax Tr

= = = = = = = = = = = = = = =

SDOF Time domain harmonic loading function, P(t) = Real [ P(ω)eiωt ] SDOF frequency domain complex harmonic loading function SDOF harmonic loading amplitude SDOF static displacement SDOF (magnitude of the) dynamic amplification factor SDOF (magnitude of the) dynamic amplification factor at resonance when ω = ωn SDOF maximum (magnitude of the) dynamic amplification factor when ω = ωn(1-2ζ2)1/2 SDOF complex displacement response function (FRF), F(ω) = D(ω)(p0/k)e−iθ SDOF transfer function, H(ω) = D(ω)(1/k)e−iθ SDOF complex displacement response function at resonance, Fresonant = Dresonant(p0/k)e−iθ SDOF complex maximum displacement response function, Fmax = Dmax(p0/k)e−iθ SDOF time domain displacement response, u(t) = Real [ F(ω)eiωt ] SDOF time domain displacement response at resonance, u(t) = Real [ Fresonant eiωt] SDOF time domain maximum displacement response, u(t) = Real [ Fmax eiωt] SDOF transmissibility of displacement, acceleration or force

Modal Frequency Domain Loading and Steady-State Response Notations {P(t)} = {P(ω)} = Pi(ω) = p0i = p0i/Ki = Di(ω) = Di resonant = Di max = ξi(ω) = ξi resonant = ξi max = {u(t)} =

Time domain harmonic loading function vector, {P(t)} = Real [ {P(ω)} eiωt ] Frequency domain complex harmonic loading function vector Modal frequency domain complex harmonic loading function vector, Pi(ω) = {φi}T {P(ω)} Modal harmonic loading amplitude Modal static displacement Modal (magnitude of the) dynamic amplification factor Modal (magnitude of the) dynamic amplification factor at resonance when ω = ωni Modal maximum (magnitude of the) dynamic amplification factor when ω = ωni(1-2ζi2)1/2 Modal complex displacement response function (FRF), ξi(ω) = Di(ω)p0i/Ki e− iθi Modal complex displacement response function at resonance, ξi resonant = Di resonant p0i/Ki e− iθi Modal complex maximum displacement response function, ξi max = Di max p0i/Ki e−iθi Time domain displacement response vector, {u(t)} = Real [ [Φ]{ξ(ω)}eiωt ]

Additional Abbreviations

15


ML: Materially Linear MNL: Materially Nonlinear GL: Geometrically Linear GNL: Geometrically Nonlinear [] = matrix {} = column vector <> = row vector

16


1

INTRODUCTION

This paper serves as a guide to performing effective static and dynamic structural analyses with MSC.NASTRAN in particular, although the concepts described herein are also equally applicable to other analysis codes. A disbeliever wonders if the answer provided by a finite element analysis is correct. The question is not whether the correct answer has been obtained, but rather if the correct question was asked, for the answer will always be correct.

17


2 CONCEPTS OF COMPUTATIONAL FINITE ELEMENT STRUCTURAL ANALYSIS 2.1 Overview of the Finite Element Method 2.1.1

GL, ML Static Finite Element Elemental Formulation

The elemental stiffness formulation of the finite element describes the stiffness behavior of an element. The finite element elemental stiffness formulation describes the force-displacement relationship of a finite number of degrees of freedom of the element. This relationship can be formulated by one of two general methods as described below. 2.1.1.1

The Principle of Virtual Displacements of The Principle of Virtual Work (Equivalent to the Variational Method or The Principle of Minimum Potential Energy)

The stiffness of a linear system is based on the stiffness at the initial undeformed state. Define state A as the initial undeformed state. The variation of displacement within a finite element can be presented as a function of the matrix of shape functions [N] and the discrete nodal degree of freedom displacement vector {d} as {y} = [N]{d} Vector {y} describes the general displacement function (interpolation function) within the finite element, {d} is the unknown nodal DOFs and [N] are their corresponding shape functions. The general strain vector {ε} in terms of {d} can then be derived as the strain is some derivative function of the displacement function and hence the nodal DOFs {d} {ε} = [BA]{d} The general stress vector {σ} can then be established in terms of the strains and hence be expressed in terms of the DOFs {d} amongst other terms {σ} = [DA][BA]{d} + {σ}i − [DA]{ε}i The second term is due to the initial stresses (such as residual stresses within the element) and the third term is the initial strains due to temperature shrinkage or lack of fit. Two equivalent fundamental theorems of structural analysis are the principle of virtual displacements (virtual work) and the principle of minimum potential energy. These theorems provide the fundamental Newton’s equilibrium equations for the finite element. The principle of virtual displacements (virtual work) states that a structural system is in equilibrium in its deflected configuration if the external work performed by the applied loading over any possible infinitesimal displacement mode is equal to the internal work performed by the component forces over the corresponding compatible infinitesimal deformations. In other words, a system is in equilibrium when the external work done equates the internal work. The equivalent principle of minimum potential energy states that a structural system is in equilibrium in its deflected configuration if its total potential energy (V), consisting of the system strain energy (U) and the loading potential energy (-W), is stationary with respect to any infinitesimal variation in the possible deformation modes. For a finite element, the equilibrium equation is thus derived by equating the external work to the internal energy for a virtual displacement set. (Virtual Nodal Disp) x (Real Nodal Forces) + (Virtual General Disp) x (Real Distributed Forces) = (Virtual Strains Or Deformations) x (Real Stresses Or Actions)

18


δ{d} {f } + Τ

∫ δ{y} {b}dΩ = ∫ δ{ε} {σ}dΩ Τ

T

Ω

Ω

where {f} is the nodal force vector and {b} is the distributed body forces within the finite element. We have however established that

{y} = [ N ]{d} hence {y}T = {d}T [ N ]T {ε} = [B A ]{d} hence {ε}T = {d}T [B A ]T {σ} = [D A ][B A ]{d} + {σ}i − [D A ]{ε}i hence

δ{d} {f } + Τ

∫ δ{d} [ N] {b}dΩ = ∫ Τ

Ω

T

Ω

δ{d}T [ B A ] T [ D A ][ B A ]{d}dΩ +

∫

Ω

δ{d}T [ B A ] T {σ}i dΩ −

∫

Ω

δ{d}T [ B A ] T [ D A ]{ε}i dΩ

The above expression is valid for any virtual displacement δ{d}. Choosing unity virtual displacements we arrive at the elemental equilibrium equations

[

] {∫ [B

{f } = ∫Ω [B A ]T [D A ][B A ]dΩ {d} +

Ω

} {∫ [B

] {σ}i dΩ −

A T

Ω

} {∫ [N] {b}dΩ}

] [D A ]{ε}i dΩ −

A T

Τ

Ω

This is the expression that is set up for each and every element. If the nodal force vector {f} is known, then the only remaining unknown within these equations are the nodal displacement vector {d}. Note that we have defined [B] the strain matrix, {σ}i = the initial stresses, [D] the material constitutive matrix, {ε}i = the initial strains, [N] = shape functions matrix, {b} = the elemental (external) body loads and of course {d} = nodal element displacement in element axes. To summarize the terms in the above elemental static equilibrium equation expression (i) (ii) (iii)

the term on the LHS is the nodal force vector in element axis the first term on the RHS is the instantaneous stiffness matrix the second, third and fourth terms on the RHS are the so-called fixed end forces

We note that the choice of the shape functions [N] affects the accuracy of (i) (ii)

the elemental instantaneous stiffness matrix the fixed end forces

The important concept to grasp is that geometrically linear (GL) finite elements have linear strain-displacement relationships i.e. the [BA] matrix would be constant and thus independent of the nodal displacements {d}. Materially linear (ML) finite elements have linear stress-strain relationships i.e. the [DA] matrix would be constant and thus independent of the strain vector {ε}.

19


2.1.1.2

The Method of Weighted Residuals

We have seen that the principle of virtual displacements or the principle of minimum potential energy (variational approach) can be used to establish the element stiffness matrix. The shape function [N] is applied to the variational statement in the discretization. Another method of establishing the elemental stiffness matrix is the method of weighted residuals. Here, instead of applying the shape functions [N] to the variational statement, it is applied to the so-called weak statement. The weak statement is a perfectly equivalent integral form of the strong statement which is the governing Newton’s differential equation representing the equilibrium of the element internal and external forces. The weak statement of a differential equation (strong statement) can be stated as

∫ v(Differential Equation )dΩ + v(Natural Boundary Conditions of the Differential Equation) = 0 Ω

for any function of v and v. The weak statement is perfectly equivalent to the strong statement. The shape function [N] is applied to the differential equation. Any shape function [N] that satisfies the strong statement also satisfies the weak statement. The functions v and v are the weighting function for the error in the differential equation and the natural boundary conditions respectively. The weak statement is perfectly equivalent to the strong statement if the weak statement is satisfied for any weighting functions whatsoever. In words, the weak statement states that the residual errors in the approximation of the original differential equation and the natural boundary condition weighted by the weighting functions are zero, hence the name weighted residual methods. This does not mean that the error in the strong statement is zero, as there will still be approximations in the shape functions [N]. On top of that, usually, the weak statement will not be satisfied for all weighting functions. The choice of the finite weighting functions define the various different methods of weighted residuals. Two common methods within the method of weighted residuals are the sub-domain collocation method and the popular Galerkin method (which is equivalent to the variational approach). The sub-domain collocation method divides the geometric domain into as many sub-domains as there are DOFs with the weighting functions having a value of unity in a particular sub-domain and zero in all other sub-domains leading to one equation from the weak statement. The weighting functions are also put to unity at other sub-domains in turn, leading to a set of simultaneous equations which formulate the elemental stiffness matrix. In the Galerkin approach, the weighting functions are identical to the shape functions. Since there are as many shape functions as there as DOFs, each shape function is applied to the weak statement for an equation. This leads to a set of simultaneous equations which formulate the elemental stiffness matrix. The Galerkin approach is actually exactly equivalent to the variational approach.

20


2.1.2

GL, ML Static Finite Element Global Formulation

The following describes the assembly of the element stiffness matrices towards the formulation of the global system stiffness matrix by the use of the equilibrium, compatibility and constitutive laws. We have shown that the elemental equilibrium equations are

[

] {∫ [B ] {σ} dΩ}− {∫ [B ] [D ]{ε} dΩ}− {∫ [N] {b}dΩ} ] {σ} dΩ}− {∫ [B ] [ D ]{ε} dΩ}− {∫ [ N ] {b} dΩ}

{f } = ∫Ω [B A ]T [D A ][B A ]dΩ {d} +

[ ]

= k AE {d} +

{∫ [B Ω

A T

A T

i

Ω

A T

A T

i

Τ

A

i

Ω

Ω

Τ

A

i

Ω

Ω

Inherent within this expression is the material constitutive law. This expression is computed for each and every element in the element axes system. These contributions make up the nodal equilibrium equations at each and every node. In order to assemble that, we again employ the principle of virtual displacements

δW = δ{d} {f } (for all δ{U}) T

 ∂W   ∂{d}    =  ∂{U}  ∂ U 

T

{f }

{P} = [T]T {f } or the principle of minimum potential energy

Total Potential Energy, V = U + (− W) δV = δU − δW = 0

(for all δ{U})

1 T {d} [k ]{d} (for linear elastic material) 2 T T δU = δ{d} [k ]{d} = δ{d} {f } U=

δV = δ{d}T {f } − δW = {0}  ∂V   ∂{d}  For equilibrium,   =  ∂{U}  ∂ U 

T

 ∂W   ∂{d}    =  ∂{U}  ∂ U 

T

{f } −  ∂W  = {0}  ∂{U} {f }

{P} = [T ] T {f } Both theorems result in the nodal equilibrium equations {P} = [TA]T{f} where {P} is the nodal external force vector in global axes system, {f} is the elemental nodal force vector in the element axes system and [T] is the transformation matrix. The vector {P} is thus the user-specified external loads which are known. The transformation matrix [T] transforms the elemental contribution to the static equilibrium equations such that compatibility is ensured. Also note that the displacement DOFs need also be transformed to ensure compatibility {d} = [TA]{U}

21


We thus obtain the nodal static equilibrium equations in the global axes system {P} = [T A ] T {f }

A T

[ ]

{[∫ [B

]

{∫ [B ] {σ} dΩ}− {∫ [B ] [D ]{ε} dΩ}− {∫ [N] {b}dΩ} = [T ] [k ][T ]{U} + [T ] {∫ [B ] {σ} dΩ}− [T ] {∫ [B ] [D ]{ε} dΩ}− [T ] {∫ [ N] {b} dΩ} = [K ]{U} + [T ] {∫ [B ] {σ} dΩ}− [T ] {∫ [B ] [D ]{ε} dΩ}− [T ] {∫ [ N] {b} dΩ} = [T A ] T

A E

Ω

A E

] [D A ][B A ]dΩ [T A ]{U} +

A T A

A T

[ ]

A T

A T

A T

Ω

i

A

Ω

A

Ω

Τ

A T

i

Τ

A T

i

Ω

A T

Τ

A

Ω

A T

i

i

Ω

A T

i

A T

Ω

A T

A T

Ω

Ω

as K AE = [T A ] T k AE [T A ]

The first term on the RHS in the nodal static equilibrium equation expression is the global instantaneous stiffness matrix. The second, third and fourth on the RHS are the fixed end forces in the global axes system. Note that the only unknowns in this expression are the global nodal displacement DOFs {U}. Hence in a linear static solutions scheme, this expression is solved for {U} after the essential boundary conditions are applied using a simultaneous equation solving algorithm such as Gaussian Elimination. The stiffness matrix prior to application of the essential boundary conditions is known as the initial stiffness matrix whilst that after the application of the essential boundary conditions is known as the final stiffness matrix. The essential boundary conditions may be zero (constraints) or non-zero (settlement or enforced displacement). Applying zero essential boundary condition effectively refers to deleting both the row and column associated with the constrained DOF. Applying a non-zero (settlement) essential boundary condition refers to deleting the row but not the columns associated with the DOF with the settlement. The deletion of the row indicates that the additional equation defining the DOF as an unknown is not utilized within the simultaneous solver. And by not deleting the column, the remaining equations utilize the known displacement value, which becomes a part of the fixed end forces when the term is brought over the loading side of the equations. Hence the specification of the enforced displacement always requires the specification of a constraint to delete the row (SPC entry in MSC.NASTRAN) and the specification of an enforced displacement to account for the known displacement value for the column (SPCD entry in MSC.NASTRAN). For example if the following is the initial stiffness matrix where f now denotes the fixed end forces  P1   f 1   K 11  P  f   K  2   2   21  − =  P3  f 3   K 31 P4  f 4   K 41

K 12

K 13

K 22 K 32 K 42

K 23 K 33 K 43

K 14   U 1  K 24   U 2    K 34   U 3   K 44   U 4 

and if the displacement U1 is a settlement or an enforced displacement, and U2 is a constraint, then the final stiffness matrix  P1   f 1   K 11  P  f   K  2   2   21  − =  P3  f 3   K 31 P4  f 4   K 41

K 12

K 13

K 22 K 32 K 42

K 23 K 33 K 43

K 14   U 1  K 24   U 2    K 34   U 3   K 44   U 4 

giving

 P3  f 3  K 31 U 1   K 33  − − = P4  f 4  K 41 U 1   K 43

K 34   U 3    K 44   U 4 

22


Notice the settlements now contribute to the fixed end forces. This expression is solved simultaneously for the unknown displacements U3 and U4. Solving these final stiffness static equilibrium equations simultaneously then, effectively produces the deformed configuration of the structure. Finally, element stress recovery is performed utilizing {σ} = [DA][BA]{d} + {σ}i − [DA]{ε}i The reactions (obtained for both zero and non-zero essential boundary conditions) are obtained from the deleted rows of the initial stiffness matrix. For the above example, the reactions P1 (at the settlement) and P2 (at the zero constraint) are  P1   f 1   K 11  − = P2  f 2   K 21

K 12 K 22

K 13 K 23

 U1  K 14   U 2    K 24   U 3   U 4 

The reaction at the enforced displacement constrained should be checked after an analysis to ensure that the forces required to effect this displacement are realistic. Note that a static analysis can be solved with solely applied displacements, i.e. loads are not mandatory, as long as the 6 rigid-body modes are constrained. Again, it is important to grasp the concept that in geometrically linear (GL) global element stiffness formulations, the transformation matrix [TA] is constant and thus independent of the global displacement vector {U}.

23


2.1.3

GNL, MNL Static Finite Element Elemental Formulation

The variation of displacement within a finite element can be presented as a function of the matrix of shape functions [N] and the discrete nodal degree of freedom displacement vector {d} as {y} = [N]{d} Vector {y} describes the general displacement function (interpolation function) within the finite element, {d} is the unknown nodal DOFs and [N] are their corresponding shape functions. The general strain vector {ε} in terms of {d} can then be derived as the strain is some derivative function of the displacement function and hence the nodal DOFs {d} {ε} = [B]{d} One of the differences with a nonlinear finite element stiffness formulation lies in the elemental strain expression {ε} which is no longer linearly related to the nodal displacement DOFs {d}. Hence the strain matrix [B] is no longer constant but instead a function of the nodal displacement vector {d}. This has further repercussions that will become apparent. The general stress vector {σ} can then be established in terms of the strains and hence be expressed in terms of the DOFs {d} amongst other terms {σ} = [D][B]{d} + {σ}i − [D]{ε}i The second term is due to the initial stresses (such as residual stresses within the element) and the third term is the initial strains due to temperature shrinkage or lack of fit. For material nonlinearity, the constitutive matrix [D] is also dependent upon the strains {ε} which in turn is dependent upon the nodal displacement vector {d}. For a variational finite element, the equilibrium equation is thus derived by equating the external work to the internal energy for a virtual displacement set or by minimizing the total potential energy (note that these theorems are equally applicable for nonlinear systems as they are for linear systems) V=U−W δV = δU − δW = 0 δV =

for equilibrium

∫ δ{ε} {σ}dΩ − δ{d} {f } − ∫ δ{y} {b}dΩ = 0 Τ

T

Τ

Ω

Ω

where {f} is the nodal force vector and {b} is the distributed body forces within the finite element. We have however established that

{y} = [ N ]{d} hence {y}T = {d}T [ N ]T {ε} = [B]{d} hence {ε}T = {d}T [B] T {σ} = [D][B]{d} + {σ}i − [D]{ε}i hence

δ{d} {f } + Τ

∫ δ{d} [ N] {b}dΩ = ∫ Τ

Ω

T

Ω

δ{d}T [ B] T [ D][B]{d}dΩ +

∫

Ω

δ{d}T [ B] T {σ}i dΩ −

∫

Ω

δ{d}T [ B] T [ D]{ε}i dΩ

The above expression is valid for any virtual displacement δ{d}. Choosing unity virtual displacements we arrive at the elemental equilibrium equations

[

] {∫ [B] {σ} dΩ}− {∫ [B] [D]{ε} dΩ}− {∫ [N] {b}dΩ}

{f } = ∫Ω [B]T [D][B]dΩ {d} +

T

Ω

Τ

T

i

Ω

24

i

Ω


This is the expression that is set up for each and every element. If the nodal force vector {f} is known, then the only remaining unknown within these equations are the nodal displacement vector {d}. Note that we have defined [B] the strain matrix, {σ}i = the initial stresses, [D] the material constitutive matrix, {ε}i = the initial strains, [N] = shape functions matrix, {b} = the elemental (external) body loads and of course {d} = nodal element displacement in element axes. To summarize the terms in the above elemental static equilibrium equation expression (i) (ii) (iii)

the term on the LHS is the nodal force vector in element axis the first term on the RHS is the instantaneous stiffness matrix the second, third and fourth terms on the RHS are the so-called fixed end forces

We note that the choice of the shape functions [N] affects the accuracy of (i) (ii)

the elemental instantaneous stiffness matrix the fixed end forces

This elemental static equilibrium expression seems exactly identical to that of the linear finite element. However, there are inherent fundamental differences that must be realized, i.e. (i)

Firstly, the strain matrix [B] is no longer constant but instead dependent upon the nodal displacement vector {d}, this being a characteristic of geometric nonlinearity. (ii) Secondly, the constitutive matrix [D] is not constant but instead dependent upon the nodal displacement vector {d}, this being a characteristic of material nonlinearity. (iii) Thirdly, the body loading vector {b} is also dependent upon the nodal displacement vector {d}, this also being a characteristic of geometric nonlinearity

An extremely fundamental concept to grasp is that as a result of the dependence of [B], [D] and {b} on {d}, we can no longer solve for {d} using linear simultaneous equation solving algorithms. In the linear systems, we write the expression {f} = [kE]{d} + Fixed End Forces and provided we know the applied nodal forces {f}, which we do, we can solve for {d} as the fixed end forces are independent of {d}. Now, in the nonlinear system, the equilibrium equations are nonlinear. We thus employ another technique based on the tangent stiffness in order to solve the nonlinear equilibrium equations for {d}. The stiffness matrix of the nonlinear system is no longer constant. By definition the stiffness of the system is

[k ] =  ∂{f }  



 ∂ d 

For a linear finite element, since [B], [D] and {b} are independent of {d}, the second, third and fourth terms in the elemental equilibrium equation does not feature in the stiffness expression which simply is [k ] =

[∫ [B] [D][B]dΩ] T

Ω

On the other hand, for a nonlinear finite element, there are remaining terms when the second, third and fourth terms of the elemental equilibrium equation are differentiated with respect to {d} to obtain the elemental tangent stiffness expression as shown below.

25


 ∂2V  ∂{d}∂ d

[k T ] = 

 ∂2U =  ∂{d}∂ d

     ∂2W −   ∂{d}∂ d

{

}

  

 ∂   ∂2W = [B] T {σ}  −   ∂ d   ∂{d}∂ d

 ∂{ε}  as [B] =    ∂ d 

  

 ∂[B]T   2 T  ∂{σ} {σ} −  ∂ W = [B]  +  ∂ d   ∂ d   ∂{d}∂ d

  

using the derivative of product rule

 ∂[B]T   2 T  ∂{σ}  ∂{ε}  {σ} −  ∂ W = [B]   +  ∂ ε   ∂ d   ∂ d   ∂{d}∂ d  ∂[B]T   2 T {σ} −  ∂ W = [B] [D][B] +   ∂ d   ∂{d}∂ d

  ∂{σ}  ∂{ε}   as [D] =   and [B] =     ∂ ε   ∂ d 

 ∂  ∂{ε}  T   ∂ 2 W = [B] [D][B] +    {σ} −   ∂ d  ∂ d    ∂{d}∂ d   2    2  ∂ ε = [B]T [D][B] +  {σ} −  ∂ W   ∂{d}∂ d   ∂{d}∂ d  T

  using the chain rule 

  ∂{ε}   as [B] =     ∂ d 

Hence, we can conclude that the elemental tangent stiffness matrix is

[k T ] = [k E ] + [k G ] [k E ] = ∫ [B]T [D][B]dΩ Ω

 ∂2 ε

[k G ] = ∫   Ω

∂{d}∂ d

{{σ}n

  ∂ 2 Wi   ∂ 2 Wn  + {σ}i − [D]{ε}i }dΩ −  − λ     ∂{d}∂ d   ∂{d}∂ d  

{σ} n = [D][B]{d}

It is apparent now that the stiffness of the nonlinear finite element (and by stiffness we mean the variation of resistance {f} with respect to the nodal displacement {d}) is not just dependent upon the instantaneous stiffness [kE] but also includes second order internal strain energy and external work terms so-called the differential stiffness terms due to the initial and nominal stresses within the finite element and the initial and nominal external work done on the element. To summarize, the primary differences with the nonlinear static stiffness formulation are (i)

the elemental strain {ε} have higher order (than linear) terms of the displacement DOFs {d} and hence the strain matrix [B] is no longer constant but instead dependent upon the nodal displacement vector {d}, this being a characteristic of geometric nonlinearity. Hence, firstly, the [B] term within [kE] is dependent upon the state of deflections {d} instead of being constant with respect to {d}, and secondly, the second derivative of the strain {ε} with respect to {d} is not zero thus causing the addition of a geometric stiffness that is also a function of the prestress.

26


(ii)

the constitutive matrix [D] is not constant but instead dependent upon the nodal displacement vector {d}, this being a characteristic of material nonlinearity. (iii) the elemental loading vector {b} has higher order (than linear) terms of the displacement DOFs {d}, this also being a characteristic of geometric nonlinearity. These differences produce stiffness terms that are not constant (or independent) with respect to {d} but instead dependent upon {d}. The nonlinearity of the stiffness expression thus requires the evaluation of an appropriately called tangent stiffness matrix. Elements with GNL capabilities have thus the following additional capabilities: (i) (ii)

(iii)

The instantaneous stiffness matrix [kE] is dependent upon the deflected configuration. This is because the strain-displacement relationship is nonlinear i.e. [B] would be a function of {d}. Elements with the capability of nonlinear [B] matrices are termed large strain elements. The geometric (or differential) stiffness matrix is dependent upon the state of stresses (or forces for one-dimensional finite elements) as depicted by the {σn+σi+Dεi} term where {σi} is the initial prestress and {εi} is the initial strain. Elements that are capable of modelling this effect are termed large strain elements. The geometric (or differential) stiffness matrix is dependent upon the second order variation of initial and nominal work done with respect to the local element DOFs. There will be no contribution from these terms if the applied external forces are work-conjugate with the element DOFs. By work-conjugate, we mean that these second-order work terms will produce equivalent nodal loading which are always in the direction of the local element nodal displacement DOFs {d}. GNL elements capable of modelling the ‘follower force effect’ where the force direction is dependent upon the deflected shape would make contributions to these terms as the equivalent nodal force contributions are then not work-conjugate.

Elements with MNL capabilities have the following additional capabilities: (i)

The stress-strain relationships is nonlinear i.e. [D] would be a function of {ε} which in turn is a function of the nodal displacement vector {d}

These GNL, MNL elements reduce to GL, ML elements if [B], [D] and {b} are constant in which case the stiffness matrix will not be dependent upon the state of stress (or forces for one-dimensional finite elements) or the second order work variation. The stiffness matrix then corresponds to that of the instantaneous stiffness matrix at the initial undeflected configuration state, A. GNL, MNL elements [f ] = [k T ]{d}

but cannot be solved by linear simultaneous equation solving algorithms

[k T ] = [k E ] + [k G ] [k E ] = ∫ [B]T [D][B]dΩ Ω

 ∂2 ε

[k G ] = ∫   Ω

∂{d}∂ d

{{σ}n

  ∂ 2 Wi   ∂ 2 Wn  + {σ}i − [D]{ε}i }dΩ −  − λ     ∂{d}∂ d   ∂{d}∂ d  

{σ}n = [D][B]{d} GL, ML elements

[ ]   [f ] =  ∫ [B ] [D][B ]dΩ {d} [f ] = k AE {d}

A T

Ω

A



can be solved by linear simultaneous equation solving algorithms

27


In conclusion, nonlinear finite elements have the following additional capabilities (i) (ii) (iii)

Large strain effect – Non constant instantaneous stiffness due to non-constant [B] and the effect of the geometric stiffness due to prestress and prestrain and nominal stress The follower-force effect Nonlinear stress-strain behavior

It is imperative to realize that the nonlinearity of [B] and the prominence of the element [kG] matrix both reduce when the element length L (or other dimensions for two and three dimensional finite elements) reduces. This brings us to a very important conclusion, i.e. that GL elements (small strain elements) can be used to approximate GNL element (large strain element or hyperelastic elements) force-displacement response if a sufficient number of elements are utilized to model a single structural member. This however does not mean that a GL analysis solution scheme can be employed, instead a GNL solution technique must be used as the nonlinearities are accounted for in the global behaviour and not the local element behaviour.

28


2.1.4

GNL, MNL Static Finite Element Global Formulation

The following describes the assembly of the element stiffness matrices towards the formulation of the global system stiffness matrix by the use of the equilibrium, compatibility and constitutive laws. We have shown that the elemental equilibrium equations are

[

]

{f } = ∫Ω [B]T [D][B]dΩ {d} + {∫Ω [B]T {σ}i dΩ}− {∫Ω [B]T [D]{ε}i dΩ}− {∫Ω [ N]Τ {b} dΩ}

Inherent within this expression is the material constitutive law. This expression is computed for each and every element in the element axes system. These contributions make up the nodal equilibrium equations at each and every node. In order to assemble that, we again employ the principle of minimum potential energy

Total potential energy

V=U−W

For equilibrium

 ∂V    = {0}  ∂{U}  ∂U   ∂W   −  = {0}  ∂{U}  ∂{U}  ∂{d}   ∂W    {f } −   = {0}  ∂ U   ∂{U} T

[T ]T {f } −  ∂W  = {0} as [T] =  ∂{d}   ∂ U   ∂{U} [T ]T {f } = {P} 



Replacing the elemental contributions to the nodal equilibrium equations, we can assemble the nodal static equilibrium equation, which can be written in its full glory {P} = [T ]

T

{[∫ [B] [D][B]dΩ][T]{U} + {∫ [B] {σ} dΩ}− {∫ [B] [D]{ε} dΩ}− {∫ [N] {b}dΩ}} T

Ω

T

Ω

Τ

T

i

Ω

i

Ω

Note that [T] is the transformation matrix between the element DOF system {d} to the global DOF system {U}. This transformation matrix is dependent upon the global system parameters {U}. The local element axes system changes with respect to the global element axes as it is dependent upon the position of the DOFs in the deflected configuration, a so-called Eulerian system. The equilibrium equations cannot be solved using a linear solution algorithm, as they are a set of nonlinear equations, nonlinearly related to {U}, which are the only unknowns. Of course a nonlinear simultaneous algorithm could in theory be applied, but this usually proves to be too computationally demanding, and inefficient. Hence, solutions schemes almost always utilize the tangent stiffness matrix approach. The tangent stiffness is independent of the unknowns {U}. Hence, for a small load or displacement step, the response of system can be approximated to be linear with respect to {U}. In other words, for a small load or displacement step, the response of the system will be linear and hence a linear simultaneous solution algorithm may be employed if the solution scheme is implicit. Knowing the tangent stiffness matrix, we can write that for a small change in {U} (small displacement step) or for a small change in {P} that δ{P} = [KT] δ{U} This is a linear relationship for the nonlinear problem. Hence, any solution scheme (static or dynamic) that incorporates the variation of stiffness with deformation {U} i.e. nonlinear stiffnesses requires a stepping algorithm in order to change the value of the tangent stiffness as the solution progresses. This is required as from the equation

29


above, it is apparent that a particular linear equilibrium equation that represents the nonlinear problem is valid only for a small load or displacement step. For completion, it is worth mentioning that when δ{P} is zero for a certain small δ{U}, this means that [KT] is zero. Physically, this means that the system is at an unstable equilibrium state, i.e. it is on the brink of buckling. The expression for the tangent stiffness matrix in the global system will now be presented. We know from the principle of minimum potential energy that a system is in equilibrium when the first order derivative of the total potential energy with respect to {U} is zero. The tangent stiffness of the system is the second order derivative of the total potential energy function with respect to {U}, i.e.



∂2V  ∂{U}∂ U

[K T ] = 

 ∂2U =  ∂{U}∂ U  ∂2U =  ∂{U}∂ U

     ∂2W −   ∂{U}∂ U   ∂{P}  −    ∂ U 

   as

 ∂W  {P} =    ∂{U}

But loads applied at nodes within a commercial finite element program are always in the direction of the global system throughout the analysis. This means that the nodal loading is work-conjugate with the global displacement vector {U} and thus there will be no second order variation in work. Thus the second term in the above expression is zero. Note that the second order variation of work terms due to loading within the finite elements is taken into account within the elemental formulations as described earlier. We thus arrive at



∂2U  ∂{U}∂ U

[K T ] = 

  

which states that the tangent stiffness matrix is equal to the second order variation of internal strain energy. Performing some basic calculus

{

}

 ∂  [T]T {f }   ∂ U 

[K T ] = 

 ∂{f }   ∂[T ]T  {f } = [T ]T  +  ∂ U   ∂ U 

 ∂{d}  as [T ] =    ∂ U  using the derivative of product rule

 ∂[T ]T  T  ∂{f }   ∂{d}  {f } = [T ]   +  ∂ d   ∂ U   ∂ U   ∂[T ]T  T {f } = [T ] [k T ][T ] +   ∂ U 

 ∂{f }   ∂{d}  as [k T ] =   and [T] =    ∂ d   ∂ U 

 ∂  ∂{d}  T  = [T ] [k T ][T ] +    {f }  ∂ U  ∂ U     2   ∂ d T {f } = [T ] [k T ][T ] +   ∂{U}∂ U  T

using the chain rule

 ∂{d}  as [T ] =    ∂ U 

30


To summarize global tangent stiffness matrix replacing terms from the elemental tangent stiffness matrix From above but and

 ∂2 d



[K T ] = [T ]T [k T ][T] + 

{f }

 ∂{U}∂ U

[



] {

}− {∫ [B] [D]{ε} dΩ}− {∫ [N] {b}dΩ}

{f } = ∫Ω [B]T [D][B]dΩ {d} + ∫Ω [B]T {σ}i dΩ [k T ] = [k E ] + [k G ] T where [k E ] = ∫ [B] [D][B]dΩ

Τ

T

i

Ω

Ω

Ω

 ∂2 ε

  ∂ 2 Wi + {σ}i − [D]{ε}i }dΩ −   ∂{d}∂ d  Ω  ∂{d}∂ d {σ} n = [D][B]{d}

[k G ] = ∫ 

and

for which Thus

{{σ}n

  ∂ 2 Wn  − λ   ∂{d}∂ d

  

[K T ] = [K E ] + [K G ] T where [K E ] = [T ] [[k E ]][T ] for which [k E ] = ∫ [B]T [D][B]dΩ Ω

and

 ∂2 d  {f } [K G ] = [T]T [[k G ]][T] +   ∂{U}∂ U   ∂2 ε

[k G ] = ∫ 

for which

Ω 

∂{d}∂ d

{{σ}n

and

{σ}n = [D][B]{d}

and

{f } = ∫Ω [B]T [D][B]dΩ {d} +

[

  ∂ 2 Wi + {σ}i − [ D]{ε}i }dΩ −   ∂{d}∂ d 

  ∂ 2 Wn  − λ   ∂{d}∂ d

  

] {∫ [B] {σ} dΩ}− {∫ [B] [D]{ε} dΩ}− {∫ [N] {b}dΩ} T

Ω

Τ

T

i

Ω

i

Ω

Note that we have omitted the second order variation of work due to the external nodal loadings {P} from the above tangent stiffness matrix expression, i.e.  ∂2W   ∂{P}  −  = −   ∂ U   ∂{U}∂ U 

as

 ∂W  {P} =    ∂{U}

This is because, as mentioned, the externally applied loads at the nodes are in commercial codes always workconjugate with the nodal DOFs {U}, failing which the above term must be incorporated. The second order variation of work due to loads applied on the finite elements is obviously still taken into account, namely in the terms

 ∂ 2 Wi   ∂ 2 Wn  −  − λ   ∂{d}∂ d   ∂{d}∂ d  Finally, the second-order work contribution of these elemental loadings to the internal energy of the global formulation is

 ∂2 d −  ∂{U}∂ U

{∫ [N] {b}dΩ} Τ

Ω



31


2.1.5 2.1.5.1

How Nonlinear Analysis Varies From Linear Analysis Geometric Nonlinearity

Geometric nonlinearity can be broken down into just four component, firstly nonlinearity due to the prominence of HIGHER ORDER ELEMENT STRAIN TERMS when local element deflections become large, secondly nonlinearity due to HIGHER ORDER WORK TERMS (FOLLOWER FORCE EFFECT) when global deflections become large, thirdly nonlinearity of the LOCAL TO GLOBAL TRANSFORMATION MATRIX when global deflections become large and fourthly the nonlinearity in the form of the global geometric stiffness matrix due to global PRESTRESS and large global displacements.

I.

HIGHER ORDER ELEMENT STRAIN TERMS. Higher order element strain terms have two effects upon the tangent stiffness matrix. Firstly, the local element instantaneous stiffness matrix [kE] becomes dependent upon the local element deflected configuration and not the undeflected configuration.

[k E ] = ∫ [B]T [D ][B]dΩ Ω

This is because the strain-displacement relationship is nonlinear i.e. [B] would be a function of {d} instead of being constant and corresponding to the initial undeflected state [BA] as in a linear analysis. If {d} is large, higher order terms in the strain-deflection {ε}=[B]{d} relationships become significant. Elemental small displacement theory does not produce correct results. This occurs because the inherent instantaneous stiffness of a structural element changes as its dimensions change as the analysis progresses. Elements with the capability of nonlinear [B] matrices are termed large strain or hyperelastic elements. In large strains elements, the strain matrix [B] varies with deflection {d}. Large strain effect occurs in metal forming, rubber and elastomer applications. The material could be elastic with linear [D] but still it may accommodate large strains within its elastic range, the higher order strains affecting its stiffness. Secondly, higher order element strain terms cause nonlinearity of the local element tangent stiffness with respect to local element deflections in the form of the element geometric stiffness due to prestress. In linear analysis, elemental [kG] is not accounted for.  ∂2 ε  [k G ] =  {{σ}n + {σ}i − [D]{ε}i }dΩ  ∂{d}∂ d Ω 

∫

where {ε} = [B]{d} {σ}n = [D][B]{d} An important observation is that the nonlinearity of [B] and the prominence of the element [kG] matrix both reduce when the element length L (or other dimensions for two and three dimensional finite elements) reduces. This brings us to a very important conclusion, i.e. that GL elements (small strain elements) can be used to approximate GNL element (large strain element or hyperelastic elements) force-displacement response if a sufficient number of elements are utilized to model a single structural member. The smaller dimensions of the small strain finite elements ensure that they are not distorted too much ensuring that the internal strains are not too large so as to invalidate the linear [B] relationship. It is perfectly valid to allow the small strain elements to undergo large total deformation as in rigid body motion, however its relative deformation must be small for its linear [B] relationship to be valid. The nonlinearity of the system is then accounted for in the global behaviour within the GNL solution technique and not the local element behaviour. II.

HIGHER ORDER WORK TERMS (FOLLOWER FORCE EFFECT). The follower force effect is the nonlinearity of the tangent stiffness with respect to deflections in the form of the geometric stiffness due to external forces, also known as the follower force effect. The geometric (or differential) stiffness matrix is dependent upon the second order variation of work done with respect to the local and global DOFs. The stiffness of the structure is dependent upon the magnitude and direction of the external element loads,

32


which again is dependent upon the current deflected configuration. This occurs when the applied force depends on the deformation (so-called follower force) in the case of hydrostatic loads on submerged or container structures, aerodynamic and hydrodynamic loads caused by the motion of aeriform and hydroform fluids (wind loads, wave loads, drag forces). Element loads often tend to follow the normal to the surface of the element. In linear analysis, these terms are not included.

 ∂ 2 Wi −  ∂{d}∂ d

  ∂ 2 Wn  − λ   ∂{d}∂ d

 ∂2 d   = −   ∂{U}∂ U

{∫ [N] {b}dΩ} Τ

Ω



Nodal forces and accelerations are always in the direction of freedoms and hence are work conjugate and hence linear analysis is sufficient to model these. Hence, there will be no contribution from these terms if the applied external forces are work-conjugate with the element or global DOFs. GNL elements capable of modelling the ‘follower force effect’ where the force direction is dependent upon the deflected shape would make contributions to these terms as the force is then not work-conjugate.

 ∂2W   ∂{P}  −  = −   ∂ U   ∂{U}∂ U 

as

 ∂W  {P} =    ∂{U}

In linear analysis, these terms are not included. III.

PRESTRESS. This is nonlinearity in the form of the global geometric stiffness matrix due to global PRESTRESS and large global displacements.

 ∂2 d  {f }    ∂{U}∂ U where

[

]

{f } = ∫Ω [B]T [D][B]dΩ {d} + {∫Ω [B] T {σ}i dΩ}− {∫Ω [B]T [D]{ε}i dΩ}− {∫Ω [ N]Τ {b} dΩ}

Geometric stiffening or destiffening is due to element stress, prestress and prestrain. There is a contribution to the geometric (or differential) stiffness matrix from the fact that an element would have internal stresses and forces. The stiffness of the structure is dependent upon the current magnitude and nature of the internal force actions within the structural element that is dependent upon the current deflected configuration. A tensile load within a structural element increases the stiffness (increasing its natural frequency) as it tends to return the element to its undeflected shape whilst a compressive load decreases the stiffness (decreasing its natural frequency) as it tends to amplify the deflected shape. Hence the high bending stiffness in prestressed cables where an unstressed cable will have negligible bending stiffness. Likewise is the reduction in stiffness in a compressed column. Also, the gradual prestressing of a structural element such as a thin plate that is restrained from longitudinal contraction and subject to bending causing the neutral surface to stretch and generate significant tensile stresses, which serve to stiffen the plate in bending due to the geometric stiffness. Of course, if the plate is not restrained, there will simply be longitudinal contraction and no in plane stress will be generated, a linear analysis is then often sufficient. Clearly, this longitudinal contraction when there are no restraints or the generation of in plane forces due to transverse bending when there are restraints, is only observed in a nonlinear analysis, not a linear one. Hence, if there is an element prestress {σi} or if the deflections {d} or {U} is sufficiently large to make the change in element stress {σn} prominent in affecting the stiffness as the analysis progresses, the geometric (or differential) stiffness matrix should be accounted for. In linear analysis, these terms are not included unless special techniques such as P-∆ analyses are performed. IV.

LOCAL TO GLOBAL TRANSFORMATION MATRIX. This is the nonlinearity of the transformation matrix [T] with respect to deflections {U}. If the deflections (U) are large, then it is appropriate to account for the variation of the [T] matrix with {U}. Even if the elemental strains are small (which can be the case if the finite element mesh is very fine), if the global deflections {U} are large, it is prudent to employ a nonlinear solution scheme.

33


[T] =  ∂{d}  



 ∂ U 

In linear analysis [T] is constant and is based on the initial undeflected configuration, i.e. [TA]. In geometrically nonlinear analysis, equilibrium and compatibility is satisfied in the deformed configuration whilst in geometrically linear analysis, equilibrium and compatibility is satisfied in the undeformed configuration. Further, the force transformation matrix is not the transpose of the displacement transformation matrix in geometrically nonlinear analysis whilst it is in linear analysis. Thus, since displacements are directly proportional to loads in linear analysis, results from different load cases can be superimposed, whilst that cannot be done for nonlinear analysis. Accounting for the nonlinearity of [T] is significant for large displacements and rotations in the case of cables, arches and thin plates. Consider a thin plate subjected to transverse loads. Shell elements are based on classical bending theory, which assumes that the transverse loads on a flat panel are resisted by bending alone. As a thin shell has little bending resistance a linear analysis would then predict a very large displacement, much larger than the limit of displacement/thickness ratios (often quoted from 0.3 to 1.0) for which the classical theory applies. In reality, once some deformation has occurred a thin shell can resist loads by membrane tension, which is very stiff compared with bending. Hence when we talk of small displacements for linear analysis to be valid, it should be quoted in view of the thickness of the element, not the absolute displacement magnitude. This is a geometric nonlinear effect where the load path and nature of deformation and stress field literally changes with deflections, an effect that cannot be predicted by linear analysis. This does not occur with curved panels such as cylinders under internal pressure, where the transverse load is carried by hoop stresses, in which case a linear analysis may be sufficient.

2.1.5.2

Material Nonlinearity

In nonlinear material finite elements, the stress-strain relationships is nonlinear i.e. [D] would be a function of {ε}.

  T  [B] [D][B]dΩ  Ω 

∫

In linear analysis, the stress-strain relationship is linear.

2.1.5.3

Contact and Boundary Conditions Nonlinearity

Nonlinear analysis is also able to change the boundary conditions as the analysis progresses. Contact can be simulated where two or more parts of the structure collide, slide and separate.

2.1.6

GL, ML and GNL, MNL Dynamic Finite Element Elemental and Global Formulation

Dynamic analysis formulations differ from static analysis by the fact that in general they require two additional matrices in the mass [M] and the damping [C] matrices. Assumed element interpolation functions now define the element mass, damping and stiffness matrices, i.e. employing the constitutive law. The dynamic global equilibrium equations are assembled (equilibrium law) from element contributions transformed (compatibility law) as appropriate. The general global dynamic equilibrium equations for nonlinear analyses are

[M ]δ{U&&}+ [C T ]δ{U&}+ [K T ]δ{U} = δ{P(t )} Since there can be prominent variations in the stiffness (and damping) matrices, the equilibrium equations is only valid for small time steps at a time. Hence, either an implicit or explicit time stepping algorithm must be employed to solve these equations for the unknowns, i.e. the global nodal displacement vector {U}. Finally, the element stress recovery is performed based on the nodal displacement vector and the assumed interpolation function.

34


2.2 2.2.1

Static Analysis Concepts Overview of Methods of Structural Static Analyses

Methods of structural static analysis may or may not incorporate nonlinearity in the form of geometric nonlinearity and/or material nonlinearity. 1. Geometrically Linear (GL) Analysis 1.1 ML Static Analysis (The Implicit Direct Stiffness Method) 1.2 ML P-∆ Static Analysis (The Implicit Direct Stiffness Method) 1.3 ML Buckling (Linear Elastic Instability) Analysis (The Implicit Linear Eigenvalue Analysis) 1.4 MNL Plastic Collapse Analysis (The Implicit Linear Simplex Programming) 2. Geometrically Nonlinear (GNL) Analysis 2.1 ML Buckling Analysis (The Implicit Nonlinear Eigenvalue Analysis) – Not feasible practically 2.2 ML/MNL Static and Buckling Analysis (The Implicit Tracing The Equilibrium Path Method, The Implicit Time Integration Method Employing Dynamic Relaxation or The Explicit Time Integration Method Employing Dynamic Relaxation) λ

ML, GL Static Analysis ML, GL Buckling Analysis λECR ML, GL P-∆ Static Analysis

ML, GNL Static and Buckling Analysis (Tracing Equilibrium Path or Implicit or Explicit Time Integration with Dynamic Relaxation) MNL, GL Plastic Collapse Analysis λP MNL, GNL Static and Buckling Analysis (Tracing Equilibrium Path or Implicit or Explicit Time Integration with Dynamic Relaxation) λF

MNL, GL Elasto-Plastic Collapse Analysis λE

U Static Analysis Methods GL: Geometrically Linear GNL: Geometrically Nonlinear ML: Materially Linear MNL: Materially Nonlinear

35


2.3

Dynamic Analysis Concepts

2.3.1 2.3.1.1

Overview of Methods of Structural Dynamic Analyses Modal Analyses

The modal properties of linear systems can be ascertained by either one of the following methods: (i) (ii) (iii)

2.3.1.2

ML, GL real modal (eigenvalue) analysis SOL 103 to establish the modal frequencies, real modal mass (and modal stiffness) and the real mode shapes ML, GL complex modal (eigenvalue) analysis SOL 107 to establish the modal frequencies, modal damping, complex modal mass (and complex modal stiffness) and the complex mode shapes ML, GL time domain implicit (SOL 109, SOL 112 or SOL 129) or explicit (LS-DYNA) impulse analysis to excite the modes of interest. The duration of the impulse must be sufficiently long (td/T1 > ~0.4) to excite the first fundamental mode, which is usually of concern. This would result in a response that includes the first fundamental mode and most likely higher modes as well. The first fundamental mode is readily ascertained from inspection of the response time history curve at any node. Higher natural frequencies can also be ascertained by performing an FFT on the response curve.

Forced Response Analyses

The methods of calculating forced dynamic response in MSC.NASTRAN are particularly of concern. Dynamic forced response analyses can be performed in the frequency or the time domain. It is important to understand the components of the result solved for by NASTRAN from the different forced response solution schemes. In general, there are two components of response, i.e. (i) (ii)

the starting transient, and the steady-state response

The excitations that contribute to the above components of response are (i) (ii)

the initial conditions, contributing to the starting transient the steady-state force, contributing to both the starting transient and the steady-state response

Forced Response Analysis Modal Frequency Direct Frequency Modal Transient Direct Transient

MSC.NASTRAN Forced Response Analysis Initial Conditions Starting Transient Response No No No No No Yes Yes Yes

Steady State Response Yes Yes Yes Yes

Methods of calculating the forced response generally depend on the nature of the excitation function. Dynamic analysis can be performed in either the time domain or the frequency domain. Time domain dynamic analyses include both transient and steady-state response, whilst frequency domain dynamic analysis only computes the steady-state response. The types of excitations and the corresponding solution methods are: (i)

ML, GL Deterministic periodic harmonic long duration excitations; The starting transient is insignificant compared to the steady-state response. Forced response (steady-state) is performed in the frequency domain using SOL 108 or SOL 111. Damping estimates ARE crucial.

36


(ii)

ML, GL Deterministic periodic non-harmonic long duration excitations; The starting transient is insignificant compared to the steady-state response. A periodic (of period T) function that is not necessarily harmonic can be expressed as a summation of an infinite number of sine and cosine terms, i.e. a Fourier Series. Forced responses (steady-state) are performed in the frequency domain using SOL 108 or SOL 111 with these individual harmonics (with the correct amplitudes and phase differences) as the excitations. The total steady-state response is thus the summation of the responses of the individual harmonics. Damping estimates ARE crucial.

(iii)

ML/MNL, GL/GNL Deterministic non-periodic short duration impulse (a.k.a. blast) excitations with subsequent wave propagation; The starting transient is significant as is steady-state response. Sources of excitation include the start up of rotating machines (not the continuous functioning) being brought to speed passing through various frequencies, but not sustaining any as to cause steady-state conditions. Other sources include sudden impulse (force applied is the rate of change of momentum of relatively small mass compared to mass of structure) or blast excitations. Forced response (starting transient and steady-state) is performed in the time domain using SOL 109, SOL 112 or SOL 129. Material properties that are not only nonlinear with the level of load but also the rate of loading (strainrate) may have to be incorporated in these sudden impulse analyses. Damping estimates ARE NOT crucial.

(iv)

ML, GL Random stationary (and ergodic) long duration excitations; This is the random equivalent of the deterministic periodic (harmonic or non-harmonic) long duration excitation. The starting transient is insignificant compared to the steady-state response. Forced response (steady-state) is performed in the frequency domain using random vibration analysis (with Fast Fourier Transforms FFT) utilizing SOL 108 or SOL 111. Damping estimates ARE crucial. Forced response in the time domain using deterministic methods may not be appropriate as they will be too computationally expensive due to the long duration of the excitation and the maximum response will be governed by steady-state conditions, not by the starting transient response.

(v)

ML/MNL, GL/GNL Random non-stationary short duration impulse excitations; This is the random equivalent of the deterministic non-periodic short duration impulse excitations. The starting transient is significant as is the steady-state response. Earthquake signals can be said to fall in this category. Forced responses (starting transient and steady-state) are performed in the time domain using SOL 109, SOL 112 or SOL 129 with a set of deterministic transient excitations generated from the non-stationary random excitations and the results enveloped. Alternatively, forced response (starting transient and steady-state) is performed crudely in the time domain using response (shock) spectrum analysis. Damping estimates ARE still quite crucial. Steady-state forced response in the frequency domain may not be appropriate since the duration of excitation may not be long enough for the response of the structure to reach steady-state conditions.

(vi)

MNL, GNL Projectile (a.k.a. impact) excitations with subsequent wave propagation; Forced response (starting transient and steady-state) can only be performed in the time domain using an explicit (implicit would be too expensive because of the high nonlinearity) nonlinear time integration scheme. Sudden impulse analyses involve the specification of an initial velocity to the impacting particle placed very close to the impacted structure. The particle will travel at this constant initial velocity (since no other forces, retarding or accelerating) until impacting the structure whereby a certain percentage of the mass of the structure and the mass of the particle will interact to cause a change of momentum, i.e. an impulse. Material properties that are not only nonlinear with the level of load but also the rate of loading (strain-rate) will have to be incorporated in these sudden impact analyses. Damping estimates ARE NOT crucial.

(vii)

MNL, GNL Brittle snap or redundancy check; These include the analysis of sudden fracture of structural members from the static equilibrium configuration such as the sudden snapping of a prestressed structural cable, and evaluates the redundancy available within the structure. Forced

37


response (starting transient and steady-state) can only be performed in the time domain using an explicit (implicit would be too expensive because of the high nonlinearity) nonlinear time integration scheme. This analysis always involves a two-stage procedure. The first stage involves a static solution by a linear static method or a nonlinear static method (either Newton’s tracing the equilibrium path SOL 106, an implicit dynamic relaxation by SOL 129 or an explicit dynamic relaxation method LSDYNA) in order to obtain the deflected configuration and the stiffness of the structure in the deflected configuration KT by the prestress (prestressing of structural members such as cables contribute greatly to a large change in stiffness within the static solution and hence will require a nonlinear static method) and gravity. The second stage involves a restart into a nonlinear transient dynamic solution scheme with no additional dynamic excitation but with a change in the structure (in the deletion of a member that fails in brittle fashion simulating a redundancy check) or a change in boundary condition (to simulate the effect of the loss of a support or anchor attached to a prestressed cable etc.). An example would be the gradual prestressing of structural cable elements within a suspension bridge or a cable prestressed tower until a static solution (by SOL 106, implicit SOL 129 or explicit LS-DYNA) is achieved. The cables can be prestressed using a gradual temperature load case (or a gradual enforced displacement on the cable anchorage points) plus gravitational loads until the correct level of prestress is achieved (by SOL 106, implicit SOL 129 or explicit LS-DYNA). Then with a restart into an explicit transient dynamic scheme of LS-DYNA, the boundary condition supporting the cable is released or a cable element is deleted, causing the structure to experience an out-of-balance of forces and hence vibrate to a new static equilibrium configuration. Damping estimates ARE NOT crucial.

2.3.2

Nature of Trial Solution in Harmonic Frequency Vibrations Complementary Function (Starting Transient) SDOF Modal MDOF λt N/A u(t) = Ge G = G1 + iG2 λ = α + iω

Direct MDOF N/A

Particular Integral Function SDOF u(t) = F(ω)eiωt F(ω) = F1(ω) + iF2(ω)

Modal MDOF {u(t)} = [Φ]{ξ(ω)}eiωt {ξ(ω)} = {ξ1(ω)} + i{ξ2(ω)}

38

Direct MDOF {u(t)} = {F(ω)}eiωt {F(ω)} = {F1(ω)} + i{F2(ω)}


2.4

Static and Dynamic Analyses Sequences

A dynamic analysis is always performed about the static equilibrium position. That is to say, the structure should be in static equilibrium before dynamic loads are applied. To obtain the total response, a few approaches may be used.

In the first approach, valid for both LINEAR AND NONLINEAR TIME DOMAIN solutions, the static response must be added to the dynamic response if the dynamic analysis is performed about the initial undeflected (by the static loads) state with only the dynamic loads applied, hence causing the dynamic response to be measured relative to the static equilibrium position. This is because if the response is taken to be measured from this static equilibrium position, it can be shown that the static loads do not feature in the dynamic equation of motion. This enables the exclusion of static loads in the dynamic analysis. However, since the dynamic response is measured from the static equilibrium position, the total response = the dynamic response + the static response to static loads. In the second approach, valid for both LINEAR AND NONLINEAR TIME DOMAIN solutions, if the dynamic analysis is performed with the deflected static shape as initial input and the static loads maintained throughout the dynamic excitations, the total or absolute response (static and dynamic) is obtained straight away from the dynamic analysis. Hence total response = dynamic response (which already includes the static response to static loads). In the third approach, valid for LINEAR FREQUENCY DOMAIN solutions, not only that the static response has to be added separately, but also the mean of the dynamic excitation has also got to be added separately as a static response. This is because for both deterministic periodic excitations and random PSD excitations the mean of the dynamically applied force is not included in the dynamic excitations. Hence the total response = static response to mean of dynamic excitation + dynamic response + static response to static loads. Analyses Sequences Static Analysis

GL Buckling Analysis

GL Modal Analysis

None

Dynamic Analysis GL modal analysis with [KEA]

GNL (SOL 106, implicit relaxation SOL 129 or explicit relaxation LSDYNA) analysis to GL modal analysis establish [KTA] at position with [KTA] of static equilibrium A. Approximate [KTA] can be obtained by repetitive P-∆ static analysis. GL buckling None analysis with [KEA] and hence [KGKEA] GNL (SOL 106, implicit relaxation SOL 129 or explicit relaxation LSDYNA) analysis to GL buckling establish [KTA] at position analysis with [KTA] of static equilibrium A. and hence [KGKTA] A Approximate [KT ] can be obtained by repetitive P-∆ static analysis.

39

Remark Modal analysis about static equilibrium position. Performed if both static and dynamic displacements are small.

Modal analysis about static equilibrium position. Performed if static displacements are large and dynamic displacements are small such as in the analysis of cable vibrations.

Buckling analysis about static equilibrium position. Performed if both static and buckling displacements are small.

Buckling analysis about static equilibrium position. Performed if static displacements are large and buckling displacements are small such as in the analysis of systems with prestress.

GL Forced Transient Response

GL Forced Frequency Response


None

GL frequency response analysis (no static loads, only frequency dependent loads)

Forced frequency response analysis about static equilibrium position. Performed if both static and dynamic displacements are small. The dynamic response is measured from the static equilibrium position. Hence, to ascertain the total response, the static response to static loads and static response to the mean of the dynamic excitations must be superposed.

GNL (SOL 106, implicit relaxation SOL 129 or explicit relaxation LSDYNA) analysis to establish [KTA] at position of static equilibrium A. Approximate [KTA] can be obtained by repetitive P-∆ static analysis.

GL frequency response analysis with [KTA] (no static loads, only frequency dependent loads)

Forced frequency response analysis about static equilibrium position. Performed if static displacements are large and dynamic displacements are small. The dynamic response is measured from the static equilibrium position. Hence, to ascertain the total response, the static response to static loads and static response to the mean of the dynamic excitations must be superposed.

None

GL transient response analysis (no static loads, only transient loads)

Forced transient response analysis about static equilibrium position. Performed if both static and dynamic displacements are small. The dynamic response is measured from the static equilibrium position. Hence, to ascertain the total response, the static response to static loads must be superposed.

GL transient response analysis with [KTA] (no static loads, only transient loads)

Forced transient response analysis about static equilibrium position. Performed if static displacements are large and dynamic displacements are small. The dynamic response is measured from the static equilibrium position. Hence, to ascertain the total response, the static response to static loads must be superposed.

GL transient response analysis with [KTA] and initial dynamic displacements as the converged static displacements (with constant with time equivalent dynamic static loads, and the transient loads)

Forced transient response analysis about initial undeflected by static loads position i.e. the absolute response. Performed if static displacements are large and dynamic displacements are small. The response is the absolute response, i.e. includes both the static and dynamic response.

GNL (SOL 106, implicit relaxation SOL 129 or explicit relaxation LSDYNA) analysis to establish [KTA] at position of static equilibrium A. Approximate [KTA] can be obtained by repetitive P-∆ static analysis. GNL (SOL 106, implicit relaxation SOL 129 or explicit relaxation LSDYNA) analysis to establish [KTA] at position of static equilibrium A and the converged static displacements. Approximate [KTA] and the converged static displacements can also be obtained by repetitive P∆ static analysis.

40

GNL Forced Transient Response


Forced transient response analysis about static equilibrium position. Performed if static displacements are small and dynamic displacements are large. The dynamic response is measured from the static equilibrium position. Hence, to ascertain the total response, the static response to static loads must be superposed. This should not be performed. The structure eventually vibrates about its static equilibrium position, albeit in a while. However, by applying the static loads together with the dynamic loads can cause dynamic amplification that is unrealistic. The static loads should not cause any dynamic effects (if that happens, nonlinear materials in the model may yield prematurely), because by its very definition, the static loads are static i.e. applied over an infinitely long duration. Instead, the static loads should be applied by SOL 106, implicit relaxation SOL 129 or explicit relaxation, then only dynamic analysis be performed.

None

GNL transient response analysis (no equivalent static loads, only transient loads)

None

GNL transient response analysis with constant with time equivalent dynamic static loads, and the transient loads)

GNL (SOL 106, implicit relaxation SOL 129 or explicit relaxation LSDYNA) analysis to establish [KTA] at position of static equilibrium A and the converged static displacements. Approximate [KTA] and the converged static displacements can also be obtained by repetitive P∆ static analysis.

GNL transient response analysis with [KTA] and initial dynamic displacements as the converged static displacements with (with constant with time equivalent dynamic static loads, and the transient loads)

Forced transient response analysis about initial undeflected by static loads position i.e. the absolute response. Performed if both static and dynamic displacements are large. The response is the absolute response, i.e. includes both the static and dynamic response.

Note that when restarting a transient analysis from a nonlinear static analysis (SOL 106, implicit relaxation SOL 129 or explicit relaxation LS-DYNA), the static loads which have been applied must be maintained throughout the transient phase in order to preserve the correct stiffness and the correct static equilibrium at the deflected static equilibrium position. Hence, when a transient phase dynamic analysis follows a dynamic relaxation analysis, it is prudent to define two curves for the static loads or prescribed motions, one ramped from zero to the static value in the dynamic relaxation phase and the other maintained at the same static throughout the transient dynamic analysis phase. Transient analysis is usually performed after a static solution has been achieved either by SOL 106, implicit relaxation SOL 129 or explicit relaxation LS-DYNA. The only benefit of performing dynamic relaxation prior to a transient analysis is that the structure would reach its static equilibrium position quicker before the transient phase takes place. In dynamic relaxation, the damping applied very large, in the order of about 5% of critical, whereas in the transient phase, the structure is very much under-damped. But even if the transient analysis were to be performed without dynamic relaxation, the structure would eventually vibrate about its static equilibrium position, albeit in a while as long as the static gravitational loads are applied. Hence of course, if dynamic relaxation is employed, after the dynamic relaxation phase, the static loads should be maintained throughout the transient dynamic analysis phase. It is however, theoretically incorrect to vibrate the structure from an unstressed position as in reality, the structure would be in its static equilibrium position before being subjected to transient dynamic vibration. In practice however, it can be argued that a dynamic analysis can be done without a static solution if negligible change in stiffness occurs from the static deflections (valid if static deflections are small), of course so long as it is clear that the total response must then be the addition of the static response and the dynamic response, both performed separately from the initial undeflected configuration.

41


3

METHODS OF STATIC ANALYSES

3.1 3.1.1

GL, ML Static Analysis by The Implicit Direct Stiffness Method Mathematical Formulation of Analysis λ

ML, GL Static Analysis ML, GL Buckling Analysis λECR ML, GL P-∆ ∆ Static Analysis ML, GNL Static and Buckling Analysis (Tracing Equilibrium Path or Implicit or Explicit Time Integration with Dynamic Relaxation) MNL, GL Plastic Collapse Analysis λP MNL, GNL Static and Buckling Analysis (Tracing Equilibrium Path or Implicit or Explicit Time Integration with Dynamic Relaxation) λF U


We have shown that the nodal static equilibrium equations can be written as a set of linear simultaneous equations

[ ] {∫ [B where [K ] = [T ] [k ][T

{P} = K AE {U} + [T A ]T A E

A T

A E

} {∫ [B ] [D ]{ε} dΩ}− [T ] {∫ [N] {b}dΩ} ] [∫ [B ] [ D ][B ]dΩ][T ]

] {σ}i dΩ − [T A ] T

A T

Ω

A

] = [T A

T

A T

A T

A

A

A

Τ

A T

i

Ω

Ω

A

Ω

Geometrically linear stiffness response represents only a tangential approximation to the fundamental path at the initial unloaded state. Hence, the results are valid in a range of small displacements and loading. Tangential accuracy of linear analysis depends upon the magnitude of deflection, the component forces and the applied loading. The geometrically linear equilibrium equations are solved for the unknown displacements {U}.

[ ]

Linear static K AE {U} = {P} + {Fixed End Forces}

[ ]

Linear static P - Delta K TA {U} = {P} + {Fixed End Forces} The linear static analysis is based on only the instantaneous stiffness matrix [KE] at the initial undeflected stage [KEA]. The linear static P-∆ analysis is based on the instantaneous and geometric (or differential) stiffness at the initial undeflected stage i.e. taking in to account the initial prestress and initial external load on the stiffness of the structure. The linear equations are solved simultaneous by decomposing [K] to triangular matrices, and then performing forward-backward substitution to obtain {U}. This is called the LU-decomposition method of solving linear simultaneous equations.

[K ]{U} = {P} + {Fixed End Forces} [L][U ]{U} = {P} + {Fixed End Forces} Forward Pass [ L]{y} = {P} + {Fixed End Forces } Backward Pass [U ]{U} = {y} for {U}

42

for {y}


3.1.2

Concepts of Geometric Stiffness or P-∆ (KGA From KEA) Analysis 1

The geometric stiffness or P-∆ concept will be illustrated for a simple system. A parameter that describes the prominence of the geometric stiffness for a particular system and level of loading will then be presented.

Let us assume that deflections are small (hence geometrically linear analysis) hence the rotation of the column segments can be described and any change in height can be neglected. Lateral equilibrium at the central pin shows that

Note that the spring force depends only on the deflection x, while the lateral force generated by the component of N depends on the deflection plus the initial imperfection, x + x0. Rearranging so that we have the form Stiffness x Displacement = Applied Force, we get

Geometric Stiffness 2N/L

and hence the deflection

i.e. We can see that the effect of the force N acting on this system can be seen as being like an additional stiffness term 2N/L, i.e. the geometric (aka differential) stiffness. The effect of the axial force is equivalent to an additional stiffness of value 2N / L acting laterally at the pin location. If the force is tensile (i.e. positive) then the geometric stiffness will act to increase the overall stiffness of the system. The effects on the system tend to be beneficial, the lateral deflection and hence the restraining force in the spring are reduced. Some practical examples where this type of stiffness is important are in the strings of musical instruments where the tension is adjusted to give the required natural frequency, in the blades of jet engines where the vibration characteristics are improved and the root bending 1

DALLARD, PAT. Buckling – An Approach Based on Geometric Stiffness and Eigen Analysis. Ove Arup & Partners International Ltd., London, June 1998.

43


moments reduced by the tension stiffening arising from rotation and in the antisymmetric response of unbraced cable trusses and cable nets where the ‘real’ (i.e. instantaneous, not geometric) stiffness may be negligible. On the other hand, if it is compressive then the term will be negative and the system stiffness will decrease. The effects on the system tend to be detrimental, the lateral deflection and hence the restraining force in the spring are increased. To reiterate, if N is compressive then the geometric stiffness is negative and x (the deflection) will be greater than it would be otherwise. If x is greater then the force in the spring will be greater. If we were designing that spring then we would need a stronger one than we first suspected. Therefore the effect of negative geometric stiffness (also known as the P-∆ effect) can be significant in design in some circumstances. The question is, when will this negative geometric stiffness effect be significant and when can we ignore it? One good answer to this question is to examine the dimensionless parameter λcr (also known as the critical linear elastic buckling load factor of a system).

λcr indicates the level of significance of the negative geometric stiffness (P-∆ effects) in a structure. Finding the value of λcr is effectively a linearized buckling analysis (SOL 105). Note that λcr refers to the critical linear elastic buckling load factor and not to the slenderness parameter associated with member elements such as columns and beams, which is also normally referred to by λ. In this simple pin jointed system example however, the buckling factor can easily be derived by considering the condition at which the axial compression is so great that the lateral stiffness of the system is zero. i.e. The λcr expression is independent of the lateral load and the initial lateral imperfections. Hence, in the absence of geometric stiffness considerations, there would be an abrupt bifurcation in the behavior of the system at the critical load. It is the deflection expression, presented hereafter, that the effects of the geometric stiffness considerations are seen as causing progressive amplification to lateral loads and initial lateral imperfections as the compressive load is increased until the critical load. Expressing the deflection expression in terms of Ncr

Expressing the deflection equation again, but now in terms of λcr and the deflection without geometric stiffness considerations (i.e. N = 0)

we have thus the deflection expression a function of λcr, the initial imperfection x0 and xN=0 Deflection Expression

This expression consists of two terms, the first being the amplified lateral response to lateral load when there is the geometric stiffness consideration and the second being the amplified (addition to the) lateral response to an initial imperfection when there is the geometric stiffness consideration. We say ‘addition to the’ lateral response for the second term because the deflection x is measured relative to the initial imperfection and not from the initial undeflected configuration. If there were no geometric stiffness consideration, there would be an abrupt bifurcation in the behavior of the system at the critical load Ncr. The effect of the geometric stiffness consideration are seen as causing progressive amplification to the lateral loads and initial lateral imperfections as the compressive load is increased until the critical load. It has the effect of amplifying the lateral deflection and

44


hence the spring force, or more generally, the forces in the elements resisting the lateral load. This is the P-∆ effect. The effects are apparent in practice. With the geometric stiffness consideration (and the existence of lateral loads and/or initial lateral imperfections), when a slender element is subject to axial compression, it tends to gradually bend before reaching the point of elastic instability. With the geometric stiffness consideration (and the existence of lateral loads and/or initial lateral imperfections), if a beam is subject to major axis bending, there is a tendency for the beam to twist and bend about its minor axis before lateral torsional buckling eventually occurs.

We shall investigate the amplified lateral displacement to lateral loads when there is the geometric stiffness consideration, which was shown to be

The definition of λcr is handy because it means that if λcr is a positive number greater than 1, then you have a structure that is stable, but that the structural response will be amplified by negative geometric stiffness effects. If 0 < λcr < 1, then the system is unstable. And if λcr is negative then the structural response will be attenuated by positive geometric effects. Here are some values of λcr and their corresponding amplification values.

We can see that when λcr > 10 the effects of negative geometric stiffness (P-∆ effects) are so small as to be insignificant to an engineering level of accuracy (accurate within 10%), whereas as they approach 1 they are very significant indeed. This then is the test that we were looking for. We can use the value of λcr to decide whether we need to take further account of negative geometric stiffness in our design and analysis. Generally, If λcr > 10 then P-∆ effects are insignificant and can be neglected – Perform linear analysis If 4 < λcr < 10, P-∆ effects (i.e. the geometric stiffness) should be incorporated – Perform P-∆ analysis If λcr < 4, a second order nonlinear analysis should be undertaken – Perform GNL SOL 106 analysis If λcr is 1 or less (but still positive) then amplification is infinite and some significant changes must be made to the design! It would be a mistake to be too scared of low λcr values. A very ordinary column in a building can have a λcr of < 1.6, and quite ordinary bracing systems for office buildings can have a λcr of < 4. But conversely it is not something that we can ignore and if response calculations are intended, a GNL SOL 106 must be performed. The amplified (addition to the) lateral displacement to an initial imperfection when there is the geometric stiffness consideration was shown to be

45


When λcr is large the response will be small, when λcr is small, but >1 the response will be large, and when λcr = 1 the response becomes infinite, in a similar way to the amplified lateral displacement to lateral loads due to the geometric stiffness consideration. The geometric stiffness equation for a 2D bar element is presented. Assume the bar has an axial force N (tension +) and length L, and use the local directions shown in the following diagram.

The active terms relate the geometric stiffening forces to the products of member forces and deflections. The terms in the instantaneous stiffness matrix KE depend on the Young’s modulus and Poisson’s ratio of the material, and the geometry of the element (the geometry of a beam element, for example, would include both the cross sectional properties and the length of the element). In contrast, the terms in the geometric stiffness matrix KG depend (linearly) on the forces in the element and the element geometry. The variation of the KG matrix with element forces means that any analysis using a KG matrix needs to be carried out in two stages. In the first stage the problem is solved ignoring the effects of geometric stiffening, establishing a set of element forces. These element forces are used in the second stage to construct the KG matrix. An important consequence of the variation of the KG matrix with element forces is that the KG matrix for one load case will differ from that for another. Hence while we can always refer to the instantaneous stiffness matrix as KE, we need to identify the geometric stiffness matrix by reference to the load case m for which it was derived, say KGm. The KG matrix is symmetric with connectivity similar to the KE matrix. In conclusion, the P-∆ effect is the reduction of lateral stiffness when the element is subjected to axial compression such that there is an amplified lateral response to lateral loads and an amplified (addition to the) lateral response to initial lateral imperfections (and subsequently the response of the elements providing lateral restraint) according to

1 λ cr 1 x= x + x 1 N =0 1 0 1− 1− λ cr λ cr

i.e.

x=

λ cr 1 x N =0 + x0 λ cr − 1 λ cr − 1

We have said that the deflection x is measured relative to the initial imperfection x0. If instead we present the deflection relative to the initial undeflected configuration, then we need to add x0. Hence

x + x0 =

λ cr λ cr λ −1 λ cr λ cr 1 1 x N =0 + x0 + x0 = x N =0 + x 0 + cr x0 = x N =0 + x0 λ cr − 1 λ cr − 1 λ cr − 1 λ cr − 1 λ cr − 1 λ cr − 1 λ cr − 1

x + x0 =

λ cr (x N = 0 + x 0 ) λ cr − 1

46


Thus the deflection (measured from the initial undeflected configuration) to lateral loads and initial lateral imperfections is amplified by λcr / (λcr – 1). This is a very important formula and can be applied approximately to all other general cases.

To reiterate this rather important point, the above amplification λcr / (λcr – 1) was derived for a pin jointed system. It can be shown that the same amplification results for the deflection and stress effects on other general systems. For example, a strut with an initial imperfection x0 would have a transverse deflection distribution according to x0sin(πx/L). With an axial load N, the transverse deflection would be x0sin(πx/L) [λcr / (λcr – 1)] where the buckling load is the Euler load, i.e. π2EI/L2. It follows that the bending moment distribution would be Nx0sin(πx/L) [λcr / (λcr – 1)]. For another example, a beam with a UDL would have a central deflection of 5ωL4/384EI and bending moment of ωL2/8. A good approximation to the central deflection of the beam-column with an axial load of N is (5ωL4/384EI) [λcr / (λcr – 1)] where the buckling load is the Euler load, i.e. π2EI/L2. It follows that the central bending moment is approximately (ωL2/8) [λcr / (λcr – 1)]. Generally, for response computations If λcr > 10 then P-∆ effects are insignificant and can be neglected – Perform linear analysis If 4 < λcr < 10, P-∆ effects (i.e. the geometric stiffness) should be incorporated – Perform P-∆ analysis If λcr < 4, a second order nonlinear analysis should be undertaken – Perform GNL SOL 106 analysis Note that λcr is obtained from a linearized buckling analysis (SOL 105).

The above proceedings described P-∆ analysis as a procedure by which the lateral stiffness is altered when a member is subject to an axial force, hence causing more lateral deflection and thus a greater bending moment in the member. An analogous way of looking at this is to consider an axial strut also subject to a lateral force. The lateral force causes a lateral deflection, ∆. On application of the axial force P, a bending moment equal to P.∆ will be induced in the member.

47


Performing P-∆ (KGA From KEA) Linear Static Analysis – Direct Approach

3.1.3

The governing equation is

[K ]{U} = {P} + {Fixed End Forces} + {Initial Imperfections} A T

This equation is directly analogous to the equilibrium equation derived for the simple pin jointed system above. The initial imperfections are functions of the geometric stiffness, hence

[K

A E

]

[ ]

+ K GA {U} = {P} + {Fixed End Forces} − K GA {U 0 }

Note that {U0} is a vector of initial imperfections. Because {U0} is difficult and unintuitive to define, the modal approach presented in Section 3.1.4 should be employed to perform the P-∆ analysis. To perform a P-∆ analysis, first the value of λcr is established to decide whether and how account is made of the negative geometric stiffness. If λcr > 10 then P-∆ effects are unlikely to be significant and can be neglected If 4 < λcr < 10, P-∆ effects (i.e. the geometric stiffness) should be incorporated If λcr < 4, a second order nonlinear analysis (GNL analysis SOL 106) should be undertaken Hence, only if λcr > 4 can we employ the P-∆ method for response computations. Any less, and a SOL 106 must be undertaken. To perform the P-∆ analysis, two linear static analyses are required. First, a linear static analysis is performed with the (ultimate limit state) loads m upon the instantaneous stiffness KEA to assess the distribution of axial forces in the structure. These axial forces are used to generate the geometric stiffness matrix for that load case m, KGmA which is combined with KEA to form the tangent stiffness matrix KTmA. A second linear analysis is then performed with the (ultimate limit state) loads upon the tangent stiffness KTmA to generate the P-∆ response.

{U m } = [K AE

A + K Gm

] {{P −1

m

} + {Fixed End Forces}m

[

]

}

A − K Gm {U 0 }

Note that when we are doing an ultimate limit state design, as we generally are, the axial forces that cause the P-∆ amplification need to be ultimate axial forces, otherwise we will underestimate the amplification. For this reason the loading on the structure needs to be the ultimate loading. And the results will be ultimate forces. You can’t apply characteristic loads, run the P-∆ analysis, and then factor the loads and responses up, because the amplification effect is nonlinear, as observed on the P-∆ curve below, i.e. if the initial compressive loads m were higher, then the geometric stiffness will be larger and the response will be greater. Of course, the initial loads m should be too great as to cause λcr to be less than 4. The down side of this is that each P-∆ case has to be run as an individual analysis and you can’t combine P-∆ results in the conventional way, though you can of course envelope them. λ

ML, GL Static Analysis ML, GL Buckling Analysis λECR ML, GL P-∆ ∆ Static Analysis ML, GNL Static and Buckling Analysis (Tracing Equilibrium Path or Implicit or Explicit Time Integration with Dynamic Relaxation) MNL, GL Plastic Collapse Analysis λP


MNL, GNL Static and Buckling Analysis (Tracing Equilibrium Path or Implicit or Explicit Time Integration with Dynamic Relaxation) λF U

48


The P-∆ method can be used to evaluate the fundamental buckling load factor. If the loads m were made too high, the geometric stiffness may become greater than the instantaneous stiffness, and the equations cannot be solved. Linear elastic buckling would have occurred. This means that we could in theory gradually increase the load m, run the P-∆ analysis involving the two passes each time, until the equations cannot be solved. The load at this stage is the lowest elastic buckling load. Performing this traces the above P-∆ equilibrium path. Note that the line is curved, but not flat at the onset of buckling as it is not a nonlinear method. Response calculations near the buckling load may not be accurate as λcr would be less than 4. It is much faster (and far more efficient in design) to evaluate the buckling load factor by performing an eigenvalue analysis (SOL 105). Moreover, the buckling mode shape will be clearly visible. The P-∆ method may NOT be accurate in evaluating the deflection response just before the onset of the fundamental buckling mode.

[K

A E

]

[ ]

+ K GA {U} = {Pcr } + {Fixed End Forces} − K GA {U 0 }

P-∆ analysis is only accurate when λ is large, i.e. λ > 4. Hence, if the loads p0 were scaled to just below λp0, and a P-∆ analysis undertaken, the displacement response may be inaccurate because now the load factor on λp0 is very close to unity. A nonlinear static and buckling analysis SOL 106 is recommended.

49


3.1.4

3.1.4.1

Performing P-∆ (KGA From KEA) Linear Static Analysis – Modal Approach; And Hence P-∆ Based Buckling 2 Objectives

Finding the P-∆ response by solving the P-∆ equation directly is presented in Section 3.1.3. While this method certainly works, a more intuitive modal approach may be desirable. The advantages of the modal approach are that (i) it helps to determine the most critical load combination to maximize the P-∆ effects (ii) it also allows for the imperfections (modeled to be proportional to the mode shape) to be incorporated to maximize the response and hence determine the elastic buckling capacity based on a P-∆ approach as is consistent with the BS 5950 code based Perry-Robertson method. The basis of the modal approach is the ability of the buckling mode shapes to orthogonalize the P-∆ static equilibrium equation into a set of uncoupled modal equilibrium equations, which can be solved independently for the modal responses. These modal responses can then be transformed into the physical coordinates in order to obtain the physical response. In doing so, of course there will be a certain degree of modal truncation. To obtain the same answer as that of the direct approach (without imperfections), ALL the modes (equal to the number of DOFs) need to be employed. Since it is difficult (and unnecessary) to determine which modes really contribute to the static response, we shall employ the direct approach anyway. But with the addition here, that we include the response due to the imperfections as well. The imperfections are assumed to be proportional to the mode shape. In fact, the imperfections that really need to be incorporated are that of only the lower modes (λcr < 10). Thus, the modal approach here is not intended as an alternative to the direct approach, but simply as an addition to incorporate the (modal) imperfections for a P-∆ based buckling capacity prediction in line with the code based PerryRobertson method and also to aid the selection of the critical load case. 3.1.4.2

Mathematical Formulation

A linear static analysis is first performed with load case m upon the instantaneous stiffness KEA in order to generate the geometric stiffness matrix for the particular load case KGm. The eigenvalue problem is

Note that the eigenvalue problem has to be associated with a particular load case m as the geometric stiffness matrix is dependent upon the particular load case. The eigenvalue problem is solved for the critical load factors and associated mode shapes. Solving the eigenvalue problem does not however produce a physical response. For this we consider the static equilibrium equation.

2

DALLARD, PAT. Buckling – An Approach Based on Geometric Stiffness and Eigen Analysis. Ove Arup & Partners International Ltd., London, June 1998.

50


Note that the initial imperfections is really just an additional load and is probably more illustrated if the associated terms were brought onto the RHS of the equation as –KGmx0. This equation can be solved directly as performed in Section 3.1.3. But this provides little insight into the buckled mode and hence the critical loading and pattern of imperfection that should be considered in design. As mentioned, the following eigenvalue approach is much more insightful in determining the response (deflections and forces). Representing the deflections as the summation of the responses in the individual modes

and the initial imperfections as the summation of imperfections in the individual modes (hence assuming that the shape of the imperfections is the same as the shape of the buckled mode shapes)

On substitution,

Premultiplying by the transpose of the mode shape matrix, rightly treating the imperfections as additional loads

Both KE and KGm will be diagonalized to give the modal stiffness and modal geometric stiffness

This is now a set of independent equations. Consider the ith equation as typical

Hence, the modal response

Separating the force and imperfection terms

The relationship between the modal stiffness, the modal geometric stiffness and the critical load factor λcri is Also, from the modal response expression, the modal response ignoring the geometric stiffening effects is seen to be the modal load {φi}T{f} divided by the modal stiffness

51


Hence, the modal response expression can be rewritten as Modal Deflection Expression

This modal deflection expression is analogous to the deflection expression derived in Section 3.1.2 for the simple pin-jointed column. Again, when there is geometric stiffness considerations, there is an amplified modal response to modal loads and an amplified (addition to the) modal response to initial modal imperfections (and subsequently the response of the elements providing restraint to the modal response). A consequence of the modal nature of equation of the modal deflection expression is that the overall response amplifier is difficult to predict. The amplifier 1/(1-1/λcr1) corresponding to the lowest buckling mode only applies to that part of the loading which contributes to the modal force {φ1}T{f}, different amplifiers apply to the other components of load. Hence it is unlikely that the total response will be amplified by 1/(1-1/λcr1). To illustrate this consider a simple pin ended column subject to axial load and distributed lateral load. The 1/(1-1/λcr1) amplifier would apply overall if the lateral load distribution followed the sinusoidal shape of the first buckling mode. This pattern of loading would result in zero modal forces in all modes except the first. If the lateral load distribution was uniform, say, it would generate modal forces in all odd numbered modes, each of which would have a different modal amplifier, and would result in a different overall amplifier. In theory, the physical P-∆ response can finally be obtained from

And by employing ALL the modes, the exact same response as that from the direct approach (without imperfections) will be obtained. But that is not the purpose of our exercise here. We are going to employ the direct approach anyway, this exercise is simply to aid the selection of the critical load case and for the modelling of the (modal) imperfections. 3.1.4.3

Critical Load Case Considerations

The loading used to design a structure prone to buckling must be selected with care. This is done in order to obtain the lowest possible load factor. Greater understanding of what loading may be critical can be gained from the modal deflection equation. It is useful to consider the loading on a structure as consisting of two parts applied simultaneously (a) loading which determines the value of the amplifier (via λcri) but does not contribute to the linear modal response, qi’ (b) loading which determines the value of the linear modal response qi’ (via {φi}T{f}) but does not affect the amplifier (via λcri) In a column, the axial load determines the value of the amplifier but does not contribute to the linear bending, while the lateral load determines the linear bending but does not affect the amplifier. Consider an arch prone to sway buckling and subject to asymmetric loading

52


Divide the loading into symmetric funicular and antisymmetric non-funicular components.

The funicular loading determines the axial force in the arch and hence the amplifier, but does not contribute to the linear bending. The antisymmetric loading determines the linear bending but does not affect the amplifier. In the design of buckling sensitive structures, consideration needs to be given to how these two types of loading vary against each other. The greatest overall response is likely to occur when the product of the linear response and the amplification factor is maximized. 3.1.4.4

Modelling (Modal) Imperfections

Imperfections corresponding to a particular mode shape cause response in that mode shape and not in any other. The modal response (in modal coordinates) due to imperfections is 1/(λcri–1) times the magnitude of the modal imperfection, q0i. Thus in physical coordinates, the modal response due to imperfections will be (1/(λcri–1))q0i{φ}i. Hence, the additional element forces due to imperfections can be calculated in a post-processing operation, using the additional modal responses due to imperfections simply to scale the modal element forces. It is usually sufficient to consider imperfections mode by mode, rather than combined. The value of q0i should be selected to cover the effects of all imperfections, including residual stresses and tolerance. Now, from the theoretical derivation of the Perry-Robertson buckling capacity formula, the theoretical Perry imperfection factor η is obtained η=

Ax 0 x y x y x L y = 02 = 0 = 0 Z r r L r r r

where x0 is the initial imperfection. The Perry factor η is the imperfection factor which is dependent upon the initial eccentricity, x0 and also the cross sectional properties. But BS 5950-Part 1:2000 goes a step further and requires an increase in the Perry factor due to residual stresses from rolling and welding. It thus states that the Perry factor should be η=

a (L e − L o ) 1000 ry

a = Robertson constant

The Robertson constant, a divided by 1000, i.e. a/1000 is equivalent to (x0/L)(y/r) and includes the initial imperfection, the section shape and also residual stresses. On equivalence of the two expressions for the Perry factor, an equivalent initial imperfection x0 (or rather q0i here) can be obtained as q 0i =

ry a x0 where x 0 = Ld xg y 1000

The value of the initial imperfection x0 is purposely derived to be perfectly consistent with the BS 5950-Part 1:2000 Perry-Robertson formula. We can get values for x0 that depend on the strut curve (Table 23 in BS 5950-Part 1:2000), the length of the buckled waveform Ld, and a single geometric property (ry/y) of the section that is buckling. The table below shows some appropriate values of x0 to use in common cases.

53


These values apply for the situations in the table. We have used values of ry/y that are conservative for each of the particular ranges of section type. If your structure doesn’t conform to one of the ones listed then you need to derive a value of x0 for your particular structure using the equation for x0. Don’t forget that ry/y can never be greater than 1 for a symmetrical section. The values of x0 that are given by the equation and shown in the table are derived for flexural buckling, that is buckled modes that are controlled by bending of some element or elements. When the buckling is controlled by axial extension of, for instance, a bracing system, or by shear deflections, then there is no direct method of calculating a correlation to BS 5950-Part 1:2000. In these ‘shear buckling’ situations it seems prudent to use a value of x0 = Ld/250. Mind you, don’t get too hung up on the detail of these calculations; BS 5950-Part 1:2000 says that we can ignore these effects if they contribute less than 10% of the moment in a section. By implication it is pointless to try to evaluate these effects to very high degree of accuracy. Also, the odds of the steel fabricator building the structure with an initial imperfection that exactly resembles one of the buckled mode shapes that GSA has calculated are pretty small. We still need to define the length of the waveform Ld and the deflection assumed by the solution code for the eigenvector at the middle of the waveform xg usually 1.0 for MAX normalization. In the case of the Euler strut, in mode 1, the length of the buckled waveform is equal to the length of the strut. In mode 2, L is equal to half the length of the strut, and in mode 3, L is equal to one third of the length of the strut.

In the general case however, it may be more complicated.

54


55


For real structures, when we look at a real buckling mode the first thing that we need to establish is which member, or members, is it that is a) causing the buckling and b) being affected by the buckling. When we say that a member, or members, is ‘causing the buckling’ what we mean is that we are assuming that the structure has been built with an imperfection in that member, or members (that mimics the shape of the buckled mode shape). In the case of the simple strut in example 1 this means that the strut is initially bowed. In the case of the bracing in example 14 this means that the bracing members were too long. When we say that a member is ‘affected by’ the buckling we mean that moments or forces are induced in them, under the normal structural loads, as a result of the imperfection that the structure was built with. Luckily, our definition of a buckling mode leads to the situation where the two sets of members (a) and (b) above are generally coincident. A member that the analysis code identifies as having a high curvature (or extension) becomes the one that has a curvature (or extension) as its initial imperfection. And it is no coincidence that a member with high curvature (or extension) in the buckled mode is a member that has a high moment (or axial force) in the force results for that mode. Let us call these members the primary buckling members for the mode. Spotting the primary buckling members for any given mode is made easier by looking for the maximum ‘total strain energy density’ in the structure in that mode. The total strain energy density is a value that the analysis code calculates, and will display, either as a diagram, or as a contoured value. It is, roughly speaking, defined as moment x curvature (or axial force x axial extension) divided by member area to give an energy density per meter along the beam. Since the total strain energy density is the product of the two variables that we are most interested in when we want to find the sets of members (a) and (b) above, it gives us a powerful graphical tool for highlighting which the primary buckling members are.

56


The resultant forces from each buckled mode can then be combined with the other ultimate forces in the structure (from the P-∆ analyses) to give sets of design forces for the final stress check. Note that each set of resultant buckling forces occurs because the structure was (we assume) built with a specific initial imperfection shape that corresponded to the buckled mode shape. Therefore we do not need to combine forces from one mode with forces from another since the structure cannot be built into both shapes at the same time. The sign of q0i should be taken so as to maximize the total response in terms of section utilization. Usually imperfections in the lowest buckling modes (λcr < 10) will cause the greatest additional response. Several such modes may need to be considered, each maximizing the utilization of particular sections. It is sometimes necessary to consider the effect of combining modal imperfections. The following plots show two mode shapes of the Millennium Wheel. The rim buckles under the compression induced by the prestress in the spokes. The load factors for the two modes are virtually identical, as are the mode shapes, except they are rotated such that the position of nodes and antinodes are swapped.

It would be incorrect only to consider imperfections in each mode separately, as this would suggest that the strength requirement for the rim varies around the circumference. A more general imperfection of the required magnitude can be obtained by combining the imperfections due to sinα.q02 and cosα.q03. The same amplifier applies to this combined imperfection, resulting in the same maximum response, except that the maximum can occur anywhere around the rim. This supports intuition, the rim strength should be constant around the circumference. Another such example is a long beam on elastic foundations, which has a numerous modes of very similar shape and load factor. Again, an analysis using a generalized imperfection, based on combined modal imperfections, would demonstrate that, away from the ends, the beam strength needs to be constant. Such paired or multiple modes arise because structure and loading have a high degree of symmetry. The Millennium Wheel has cyclic symmetry and the beam on elastic foundations has longitudinal repetition. 3.1.4.5

Design

It is quite normal to analyze structures assuming they remain linear elastic but then to check the member forces against plastic capacities. Provided the system is not prone to buckling, partial plasticity causes redistribution of the forces within the structure but it does not change the overall loading. To be strictly conservative when using linear buckling analysis, the member forces would need to be limited to the elastic capacities, reduced to allow for the effects of residual stresses. Codes of practice may allow for this by making the magnitude of the strut imperfection depend on whether the member is to be checked elastically or plastically. A similar allowance can be made in the proposed method by increasing the magnitude of the design imperfections.

57


The simplified overall buckling check in BS 5950-Part 1:2000 Clause 4.8.3.3 does not amplify the applied moments. While this is not conservative, it is usually argued that the effect is small. The more exact approach does include moment amplification, as does the proposed method. 3.1.4.6

Limitations

The proposed first order analysis method will not be appropriate if the shape of the structure changes significantly under the applied loading. The classic example would be very shallow arches that flatten under load and are prone to snap through buckling. The axial force in the arch would be significantly underestimated if calculated on the basis of the initial geometry, it needs to be calculated based on the reduced curvature of the flattened, loaded arch. The significance of the effect could be assessed by considering the change in geometry arising from limiting elastic strain in the arch.

58


3.1.4.7

Methodology

Thus, to perform a linearized elastic buckling analysis, the following procedure is undertaken for each ultimate state load combination. (a) P-∆: Apply ultimate limit state load case combination onto the structure (hence the load factors will be factors upon the ultimate limit state effects). Perform a P-∆ analysis; note two passes required. (b) Eigenvalue: Perform the linear eigenvalue buckling analysis (two passes required) to obtain the lowest buckling factor. If λcr1 > 10, then a linear static analysis (no P-∆ effects) may be sufficient. (c) Modify load case combination to maximize the amplification terms (by minimizing λcr i.e. by maximizing the geometric stiffness): Modify the load case combination in order to obtain an even lower buckling factor by maximizing the geometric stiffness matrix. From observation of the critical buckling mode shape, the loading that contributes to the geometric stiffness can be identified. This should be maximized to increase the geometric stiffness, and hence obtain the lowest buckling load factor. For example, for an arch this would mean identifying the load case combination causing the maximum arch compression and for a column, the maximum axial compression. Again, of course, the two passes (linear static on KEA and eigenvalue on KEA and KGA) must be performed for the eigenvalue analysis. Hence the lowest (λcri < 10) buckling load factors and associated mode shapes are obtained. Amplification terms

(d)

Modify load case combination to maximize linear response of critical mode: Modify the load case combination seeking to maximize the product of the linear response, dependant on the modal force {φ1}T{f}.

(e) (f)

Iteration: Repeat steps 1-4 until the smallest buckling load factors and largest P-∆ response obtained. Incorporate modal imperfection responses: Calculate the modal imperfection responses as

q 0i =

ry a x0 Ld where x 0 = Ld = xg y 1000 some constant

∴ q 0i =

(g)

Ld x g . some constant

for every significant mode, i.e. all modes that give rise to significant forces in the structure. This usually means the modes with λcr of less than 10. Total physical response: The total physical response will be the summation of the P-∆ case and the modal imperfection responses (of the significant modes with λcr < 10) in physical coordinates. Total response = P-∆ response +/- 1/(λcr1-1)q01 x {φ}1 Total response = P-∆ response +/- 1/(λcr2-1)q02 x {φ}2 … Total response = P-∆ response +/- 1/(λcri-1)q0i x {φ}i … … etc … until λcr ~ 10 We do not need to combine forces from one mode with forces from another since the structure cannot be built into both shapes at the same time. Envelope the results, hence incorporating the imperfections in all the modes up to λcr ~ 10.

59


(h)

Design: Perform local linear elastic (not ULS plastic) capacity checks on the enveloped response. This then becomes analogous to the code based Perry-Robertson element buckling check applied to global modes.

Let us look at a real example. The Core Terminal Building roof at Terminal 5, Heathrow, London is not only a very fine piece of structural engineering and a good example to look at. The model includes 2 rafters and a single pair of support structures. This frame spans the width of the terminal building and will be repeated 11 times to cover the length. The first overall buckling mode looks, at first sight, to be major axis buckling of the rafters (which are prestressed into compression as well as having an arched shape). It looks as though one goes up and the other goes down, with each behaving rather like the strut in example 1. However, examination of the strain energy density diagram reveals that it is the bracing in the roof plane that is the primary buckling member set, rather like example 13. The y direction sway and the major axis moments in the rafters are secondary effects. The value of Ld has therefore been taken as the distance between the centres of rotation of the two ends of the roof plane horizontal truss (as observed from the deflected shape diagram when viewed from above). And xg has been taken as the horizontal deflection of the centre of the truss relative to its two ends (as defined by those centres of rotation). The forces predicted by mode 1 are those that result from the bracing being installed with incorrect lengths. They tend to be axial forces in the bracing, but there are moments induced in the rafters as well.

The second overall mode could also have been deceptive. The primary buckling members are clearly the main rafters but what is causing the buckling? One might imagine that the structure was swaying in the east west direction because of the heavy vertical loads on the legs, as in examples 9 or 10. However a simplified model showed that the λcrit for that behaviour should be in the region of 40 rather than the value of 6 that the full model predicts. It turns out that a simple model based on the action displayed in example 11 is a much closer match to the behaviour of the full model. The rafter itself behaves rather like the strut in example 2, or indeed the beam in example 11. Therefore the appropriate value of Ld is measured from the end, to the point of contra flexure in the centre. And xg is taken as the vertical deflection of the rafter ¼ point (this is to avoid an overestimate of xg that might result if the east west movement were included). The forces predicted by mode 2 are caused by incorrect curvature of the rafters. The primary effect is moment in the rafters themselves, but there are also significant axial forces induced in the support structures.

The third mode is rather like the first in that the primary buckling members are in the roof bracing. In this case the action is a little more complex structurally. The centre bay of bracing diagonals has been omitted for visual reasons.

60


This means that imperfections in the length of adjacent bracing diagonals have a significant effect, and shear of this central bay forms the third mode. Again Ld is taken between points of rotation of the roof plane truss and xg has been measured horizontally. The forces predicted by mode 3 arise because of imperfect bracing lengths. The primary effect is axial in the bracing, but this mode also causes some rather inconvenient lateral moments in the CHSs of the support structures.

The fourth mode illustrates the need to keep our eyes open. The strain energy density diagram would lead us to think that the primary buckling members were the roof plane bracing, like in modes 1 and 3. But the deflected shape, and the bending moment diagram do not fit with this hypothesis. A simplified model confirmed that a straight rafter in compression would buckle in a very similar shape at a similar λcrit. Therefore we conclude that the mode is very like example 3. Ld is the length of the centre portion of rafter between the points of contra flexure. xg is measured vertically, relative to the vertical deflection of the points of contra flexure. In common with mode 2, the forces predicted by mode 4 are caused by incorrect curvature of the rafters. The primary effect is moment in the rafters themselves, but there are also significant axial forces induced in the support structures.

In addition to these overall modes there are plenty of modes that show buckling of only one part of the structure. In the case shown below it is the legs that are buckling. If you wanted to, you could use results from this analysis to check the capacity of the leg CHSs themselves. It would be just as valid, however, and probably much quicker, to use the code of practice for these sections. In this case Ld and xg would be just what you would expect from looking at example 1, and so are the forces.

61


3.1.5 3.1.5.1

MSC.NASTRAN Decks ML, GL Static Analysis

$ EXECUTIVE CONTROL SECTION SOL 101 $ CASE CONTROL SECTION DISPLACEMENT() = ALL/ SPCFORCES() = ALL/ OLOAD() = ALL/ ELSTRESS() = ALL/ ELFORCE() = ALL/ STRAIN() = ALL/ ESE() = ALL/ LOAD = < ID of FORCEi, MOMENTi, PLOADi, GRAV, LOAD, SPCD Cards in Bulk Data > TEMP(LOAD) = < ID of TEMP, TEMPRB, TEMPP1 Cards in Bulk Data > DEFORM = < ID of DEFORM Cards in Bulk Data > SPC = < ID of SPC Cards in Bulk Data >

The DISPLACEMENT request outputs the displacement vector

The OLOAD request outputs the applied loads vector

The applied loads are reported at the grid points, and include implicitly defined loads such as pressure or gravity.

62


3.1.5.1.1

Applied Loads

FORCE or MOMENT is used to apply a concentrated force or moment at a grid in either the basic or a userdefined coordinate system. $ BULK DATA FORCE

SID

MOMENT

SID

Grid ID Grid ID

CID CID

Scale Factor Scale Factor

N1

N2

N3

N1

N2

N3

To apply a concentrated force or moment at a grid point in or about a vector defined by two arbitrary grid points, FORCE1 or MOMENT1 is used. To apply a concentrated force at a grid point in or about a vector defined by the cross product of two vectors defined by four grid points, FORCE2 or MOMENT2 is used. To define a linearly varying element load on CBAR, CBEAM and CELBOW elements, the PLOAD1 card is used. $ BULK DATA PLOAD1

SID

TYPE SCALE X1, X2 P1, P2

EID

TYPE

SCALE

X1

P1

X2

P2

refers to direction and coordinate system basic coordinate system FX, FY, FZ, MX, MY, MZ element coordinate system FXE, FYE, FZE, MXE, MYE, MZE refers to either LE which means that the values of Xi are based on actual length of element or FR which means that the values of Xi are based on fractional distances with the length of element normalized to 1.0 the distances from end A, bounding the region where the load is applied the load factors at positions X1, X2

To apply a uniform normal pressure load on CQUAD4, CTRIA3 or CSHEAR surfaces defined by three or four grids on one or many shell elements, the PLOAD card is used. The direction of the pressure is based on the right hand rule and the ordering sequence of the grids. $ BULK DATA PLOAD

SID

Pressure

G1

G2

G3

G4

To apply uniform normal pressure load on CQUAD4, CTRIA3 or CSHEAR using element ids, the PLOAD2 card is used. The direction of the pressure is based on the right hand rule and the element grid definition order. $ BULK DATA PLOAD2

SID

Pressure

EID1

EID2

THRU

EID77

EID89

EID97

To apply a linearly varying not necessarily normal pressure load (such as hydrostatic pressure) on a surface of any two or three-dimensional elements, the PLOAD4 card is used. Note that point loads and moments on 1D elements are independent of the geometry of the element. Pressure loads (applied in stress units) on 2D and 3D elements are dependent upon the dimensions of the loaded face of the element. Line edge loads (applied in stress units) on 2D elements are dependent upon the thickness and the dimension of the loaded edge.

63


To apply acceleration forces on elements (such as force due to gravitational or centripetal acceleration), the GRAV card is used. The GRAV card is used to simulate a load resulting from the inertia of the component of system. Gravity may be one example. Another example may be the acceleration induced in a car component when the car accelerates. The inertia of the component will resist the acceleration and hence produce a force in the same way as it resists gravitational acceleration. Likewise, a centrifugal acceleration load allows rotating systems to be evaluated statically. $ BULK DATA GRAV

SID

CID

Scale Factor

N1

N2

N3

MB

The force due to acceleration is calculated by multiplying the mass matrix with the acceleration specified. To specify a gravitational acceleration of 9.81 m/s2, with the scale factor equaling 1.0, N3 = −9.81, with the vertical direction being the global Z direction. The mass definition is defined by the density on a material entry. The GRAV card cannot have the same ID as other static load types. Hence, a load combination must be specified using the LOAD bulk data entry with the ID equal to that specified by the LOAD card in the Case Control Section. The LOAD bulk data entry can be used to combine FORCEi, MOMENTi, PLOADi, GRAV, and SPCD cards. $ BULK DATA LOAD

SID

Overall Scale Factor

S1

S4

L4

…etc…

L1

S2

64

L2

S3

L3


3.1.5.1.2

Enforced Displacement

There are two methods available for specifying an enforced displacement at a component. The first method is to enter the value of the enforced displacement directly on an SPC entry. The alternate method to enforce a displacement at a component is to use the SPCD Bulk Data entry. The SPCD entry is actually a force, not a constraint, but it is used in conjunction with an SPC entry to enforce the displacement. When you use an SPCD entry, internal forces are computed that are applied to the structure to produce the desired enforced displacements. To specify a static enforced displacement at grid points, the SPCD card may be used. $ BULK DATA SPCD

SID

G1

C1

D1

G2

C2

D2

Grid points with an enforced displacement using the SPCD entry must also appear on an SPC or an SPC1 Bulk Data entry. The SPCD method of enforcing a nonzero constraint is more efficient than using an SPC entry alone when you are using multiple subcases that specify different constraint conditions. Note also that when you use an SPCD entry, the displacement values entered on the SPC entry are ignored-only the SPCD values are used. 3.1.5.1.3

Lack-of-Fit

To specify a lack-of-fit or vice versa on line elements, the DEFORM card can be used. $ BULK DATA DEFORM

SID

EID

D1

EID2

D2

EID3

D3

A positive deformation D1 refers to elongation and a negative D1 refers to a contraction (lack-of-fit). When using the DEFORM entry, you must remember that in general you are not enforcing a strain or an actual extensional length to the element. What you are doing is applying a force to the element that produces the specified extension if the element is free to expand without internal forces being generated. This computed force is added to the other forces in the model. Since most elements in your model are not free to expand, the extension value you specify may not be achieved. 3.1.5.1.4

Prestressed Member

The prestress is an element (such as a prestressed cable) can be modeled using temperature loads. The axial force generated from applying the temperature load on a line element that is totally fixed at its nodes can be calculated as follows, faxial = EAδ/L faxial = EAεstrainL/L faxial = EAεstrain where εstrain = α ∆T, α is the coefficient of thermal expansion (per °C) and ∆T is the change in temperature in °C. Note that the loads induced by the temperature are independent of the length of the element, L. However, it must be realized that the force calculated above is based on a fixed end line element. In reality and in the numerical model, the ends will in general not be fixed. Hence the element will contract with tensile temperature loading causing the force to decrease. Thus the specified ∆T will have to correspond to a force which is greater than the intended final prestress. Hence an iterative procedure is required (hence the need to perform the analysis repeatedly) until the required prestress is achieved in the final deflected configuration.

65


3.1.5.1.5

Thermal Expansion or Contraction

Thermal expansion and contraction is a structural rather than a thermal solution i.e. it is the analysis of stress and displacement due to thermal effects that is being considered, not the temperature at a point in the structure, which requires a heat transfer analysis. In fact, a heat transfer analysis can actually be used to generate the temperature profile and distribution and these results can in turn be applied as temperature loads in a thermal stress analysis. The input data required for analyzing thermal expansion is the coefficient of thermal expansion and the temperature distribution in model. The temperature data and the thermal expansion coefficients (in the material entry cards) are used internally to calculate equivalent forces and moments acting at grid points. Temperatures can be specified at grid point using TEMP cards, or at elements using TEMPRB (line elements) or TEMPP1 (shell elements). Average temperature specified directly for an element will take precedence over the temperature interpolated from the elements connected grid points. Solid elements get their temperature only by interpolation from connected grid points. Temperature load is calculated for a fixed ended member as faxial = EAεstrain where εstrain = α ∆T, α is the coefficient of thermal expansion (per °C) and ∆T is the change in temperature in °C This equivalent nodal load is only attained if the element is constrained from expanding and contracting. Note that the loads induced by the temperature are independent of the length of the element, L. However, if the elements is not constrained from expanding and contracting, then there will be a lateral deflection of faxial/k = faxial/(EA/L) = EAεstrain/(EA/L) = εstrainL which clearly is dependent upon the length of the element, L. Temperature loads are defined as follows. $ CASE CONTROL SECTION TEMP(INIT) = < ID of TEMP, TEMPD, TEMPP1, TEMPRB, TEMPF or TEMPAX Bulk Data Say 99 > TEMP(LOAD) = < ID of TEMP, TEMPD, TEMPP1, TEMPRB, TEMPF or TEMPAX Bulk Data Say 1 > $ BULK DATA TEMPD TEMPD TEMPRB

ID Say 99 ID Say 1 ID Say 1

Temperature 0.0 Temperature 0.0 EID1

TA

TB

EID2

THRU

EID100

EID200

THRU

EID300

TEMPD is to define temperatures at all grid points not given a temperature. It is good practice to define these and the initial nodal temperatures. TA and TB are the variations of temperature ∆T from the reference temperature defined by TEMP (INIT). Note also that SUBCOM cannot be used conventionally to combine temperature load cases. The following procedure is required. SUBCOM 3 combines the mechanical loads of load cases 1 and 2, but not their temperature loads. Temperature loads must thus be specified separately calling a separate TEMPi bulk data entry card, which can be made to combine the temperature loads of the load cases 1 and 2. $ CASE CONTROL SECTION SUBCOM 3 SUBSEQ = 1.0, 0.5 $ 1.0 x subcase 1 + 0.5 subcase 2 TEMP(LOAD) = < ID of TEMP, TEMPD, TEMPP1, TEMPRB, TEMPF or TEMPAX Bulk Data >

66


3.1.5.1.6

Linear Contact Definition with MPC Equations for SOL 101

Contact definitions (normal to contacting surfaces, no sliding friction) can be made within a linear static analysis (albeit using an iterative method). RBE2 elements can be defined between adjacent grids of surfaces, then a linear static analysis performed, then the RBE2s in tension deleted (as a contact cannot sustain tension), further linear static analyses performed and further RBE2 elements deleted until there are no RBE2 elements in tension within the contact interface. Although this method works, it is extremely cumbersome, as every load case will have a different contact distribution. This process can be automated far more elegantly using MPC equations in SOL 101. It uses a iterative constraint type approach. The constraints are applied to grid points or SPOINTS. The constraint ensures that: 1. The displacement (UR) cannot be negative. This is to ensure that there is no penetration. Therefore, the chosen degree-of-freedom must be perpendicular to the contact surface and positive in the opening direction. 2. The force of constraint (QR) cannot be negative. This is to ensure that there is no tension. The constraints are satisfied by an iterative technique that is built into SOL 101. The iterative process starts with a random vector. This random vector assumes certain grids to be in contact and other grids to be in an open state. A solution is obtained when all the gap constraints are satisfied, i.e., there's no penetration and no tension forces. If a limit cycle (return to a previous state) is detected during the iterations, a new random start vector is tried. This approach provides an alternate method to the use of GAP elements in SOL 106. Some experiments have shown that the cost of analysis will be about the same. The advantage is that you do not have to learn how to calculate the GAP stiffness nor how to control SOL 106. Multiple load conditions are allowed, and each will be solved separately. If the constraint is between a finite element model and a fixed boundary, then arrange to have one of the degrees-offreedom at the boundary grid points represent motion perpendicular to the boundary. A positive displacement represents motion away from the boundary. If, on the other hand, the constraint represents relative motion between two bodies, MPC equations are needed to define a relative motion degree-of-freedom, which is then constrained to have a non-negative displacement. Consider the following contact interface between two faces of the FE model UG2

UG1

Positive U Direction S0 The MPC for each and every pair of grids is defined as S = UG2 – UG1 + S0 where S is the relative motion DOF, UG2 – UG1 arranged such that a positive value indicates opening of the contact and S0 representing the initial gap opening, zero if the model interface gap is zero. The MPC is rearranged S – UG2 + UG1 – S0 = 0 To model a fixed contact interface between a surface of the FE model and for the definition of the card. a fixed boundary, simply omit U to represent a fixed boundary. G1

$ CASE CONTROL SECTION MPCFORCES() = ALL MPC = < ID of MPC Cards in Bulk Data, Say 1 > $ BULK DATA PARAM, CDITER, < Number of Iterations Allowed For Convergence > PARAM, CDPRT, YES (Requests printing of constraint violations during iterations) MPC

1 (MPC ID)

S

0

(Relative Motion SPOINT ID)

(SPOINT Component)

G1 (G1 ID)

S SUPORT


1.0

U (G1 Component)

0 (SPOINT Component)

67

1.0

G2 (G2 ID)

U (G2 Component)

S0

0

(Initial Gap SPOINT ID)

(SPOINT Component)

-1.0 -1.0


S SPOINT

S0


(Initial Gap SPOINT ID)

PARAM, CDPRT requests the printing of constraint violations (in terms of UR for negative displacements denoting overlap and QR denoting negative forces of constraints) during the iterations. The output is as follows. Negative Force in Constraint

At the end of the third iteration, 1 change still required PARAM, CDITER specifies No more iteration required, QR and UR satisfied after 4 iterations, i.e. after 4 static analyses. The number of changes (to the constraints) required at the end of each iteration is denoted by CHANGES and gradually will reduce until zero. At this stage, the contact interface is defined for the particular load case and all the linear GAP constraints satisfy both QR and UR. It must be checked that the CHANGES reduce to ZERO, otherwise the solution has not converged! PARAM, CDITER should be increased until convergence is achieved. NASTRAN will adopt the results of the final iteration irrespective of whether the solution has converged or not! Once convergence has been achieved, it is illustrative to find out the pairs of grids (or rather the SPOINT defining their relative motion) that are SHUT, i.e. in contact. This is indicated as follows.

Relative motion SPOINT ID and 1.0E+0 indicating the contact is SHUT, i.e. in contact. Finally, the intention would be to find out the value of the constraint forces. This is best found from MPCFORCES (PRINT) from the G TYPE Grid output. S TYPE SPOINT forces also correspond.

Relative motion SPOINT force.

Initial gap SPOINT force.

Force on one of the grids (note G TYPE) of the contact grid pair. One grid will show a positive value, and the other a negative value. If the FE surface contacts a fixed boundary, then there will only be one grid MFC (G TYPE) output.

The same values are also presented in the SPCFORCES output (only for SPOINTS), somewhat redundantly.

Relative motion SPOINT force.

Also note that large non-zero values for EPSILON and strain energy for the SUPORT degree of freedom can be safely ignored, as we are not performing inertia relief analysis.

Initial gap SPOINT force.

68


3.1.5.1.7

Modelling Centrifugal Force in SOL 101– Modelling Steady State Static Equilibrium Conditions

Centrifugal force is applied onto systems assumed to be in a steady-state, equivalent to static equilibrium. For instance, the forces acting on a car spinning in a test track at a certain velocity and/or acceleration can be ascertained using linear static analysis with centrifugal force as the system is in static equilibrium. Likewise the forces in components rotating in a rotating drum can be ascertained. The six rigid-body boundary conditions must of course still be applied onto the static system. The RFORCE entry is used to apply the force due to rotational velocity and/or acceleration. On the RFORCE entry, the components of a spin vector used internally to compute centrifugal forces are input. Each component of the spin vector is multiplied by the same scale factor. For instance consider the two rotating masses shown below. The masses are accelerated at constant angular acceleration of 20 rev/sec2 from 0 to 200 rev/min. The goal is to determine the CBAR axial force as a function of angular velocity.

SPC From graph, note that centrifugal forces are not linear with angular velocity, but proportional to ω2. Hence, using a SUBCOM command to scale the subcases with RFORCE entries can lead to misleading results if abused. The force of a single rotating part out-of-balance is F( t ) = F0 sin (Ωt ) where the amplitude is 4π 2 2 F0 = m.e. .n 3600 = m.e.4π 2 .f B2 = m.e.Ω 2 where F0 = centrifugal force (N) m = mass of the rotating part (unbalanced fraction) (kg) e = eccentricity of the unbalanced mass fraction (m) n = rate of rotation (speed of revolution of the unbalanced mass expressed in rev per minute) (r.p.m.) fB = operating frequency (fB = n/60) (Hz) Ω = angular velocity of the rotating part (=2πfB) (rad/s) Another interesting note is that the model really does not rotate; it is actually fixed at the center. If the constraints permitted the model to rotate, the run would fail. RFORCE is called by the LOAD case control command. $ BULK DATA RFORCE

SID

Grid ID

CID

Velocity Scale Factor A = ...rev/s

Acceleration Scale Factor RACC = 20rev/s2

69

R1

R2

R3

METHOD


Method=1 yields correct results only when there is no coupling in the mass matrix. This occurs when the lumped mass option is used with or without the ZOFFS option (see the CQUAD4 entry for a description of ZOFFS). Method=2 yields correct results for lumped or consistent mass matrix only if the ZOFFS option is not used. The acceleration terms due to the mass offset (X1, X2, X3) on the CONM2 entry are not computed with method=2. The possible combinations are

In addition, for problems with elements that have edge grid points (CQUAD8, CTRIA6, CTRlAX6, CHEXA, CPENTA, and CTETRA), correct centrifugal loads are produced only if the parameter PARAM, COUPMASS, x (where x is greater than 1), is included and Method 2 is used.

70


3.1.5.2

GL, ML P-∆ (KGA From KEA) Static Analysis

In order to perform a P-∆ static analysis, the geometric stiffness matrix must be calculated. However, because the geometric stiffness matrix is dependent upon the state of element stresses (or the forces in the elements), it is necessary to perform a static analysis without the geometric stiffness as a first pass, and then only perform another static analyses incorporating the geometric stiffness matrix. The following procedure can be adopted. Phase 1

Perform static analysis (with loads that cause the greatest negative or positive geometric stiffness) based on [KEA] but include the segyroa.v2001 alter prior to the Case Control Section in order to compute the geometric stiffness matrix [KGA] (and output into a .pch file) based on the generated element loads from the [KEA] static analysis. Phase 2

Perform static analysis with a general loading function based on [KEA] + [KGA] by including the k2gg = ktjj statement in the Case Control Section and the outputted .pch file which contains the ktjj matrix in the Bulk Data. The responses at this stage represent the P-∆ (KGA From KEA) static response to the general loading function. The method is valid when only the prestress is judged to affect the geometric stiffness such as in the compressive preload of building columns due to gravitational loads and the prestressing of extremely taut cables that sag very little under gravity but not in systems such as suspension bridges. Where lateral loads are large enough to affect the geometry of the system with prestress, then a repetitive P-∆, SOL 106, implicit dynamic relaxation SOL 129 or explicit dynamic relaxation must be employed. But in single P-∆ analysis, because cables do not have much elastic bending stiffness, the initial static preload subcase should only include the prestress and not gravity as including gravity is the same as solving two linear static problems of stiffness KEA with preload and gravity as the applied loads respectively. Clearly, in the gravity case, it is nonsensical as the cables do in reality have differential stiffness (from the prestress) to resist the gravitational force. Prestress in one direction (i.e. along the axis of cable) will cause a differential stiffness in the orthogonal direction. Gravity acts in the orthogonal direction and hence cannot be accounted for in the calculation of the prestress in this single P-∆ analysis. To quantitatively decide if gravity need not be considered in contributing to the differential stiffness of the cables, a static P-∆ analysis should be carried out, the first subcase being a SOL 101 with only the prestress as applied loads and the second subcase a P-∆ SOL 101 (i.e. utilizing the induced prestress from the first subcase to form a geometric stiffness matrix) with both the gravity and prestress included as applied loads. If the difference in the cable element forces between subcases 1 and 2 is negligible, then gravity has little influence in affecting the geometric stiffness. If there is a major difference in the cable element force, then clearly, gravity will affect the geometric stiffness and as such, a repetitive P-∆ , SOL 106, implicit dynamic relaxation or explicit dynamic relaxation must be used to converge to the true KT. Likewise, in the single P-∆ analysis of multi-storey buildings, gravity (and only gravity) acts in axis of columns to generate prestress, and the differential stiffness is computed for the orthogonal direction reducing resistance to lateral wind forces, applied in the second subcase with gravity too. The segyroa.v2001 alter computes the differential stiffness due to the prestress and also the follower force. The follower force is calculated and incorporated by the use of PARAM, FOLLOWK, YES. We know how the prestress affects the differential stiffness, namely a tensile prestress causing an increase in stiffness. The effect of the follower force on the stiffness is different. For example, for a cylinder under external pressure critical buckling load may be overestimated (even though the mode shapes are similar) in a SOL 105 and the natural frequencies in vibration may be underestimated (even though the mode shapes are similar) in a SOL 103 in the absence of follower stiffness. To the contrary, this observations are reversed in case of centrifugal loads. Centrifugal forces as a constant (static) load are applied by a Bulk Data RFORCE to any elements that have masses. The follower stiffness due to centrifugal load has the effect of lowering stiffness (although the centrifugal load tensioning effect increases stiffness), consequently lowering natural frequencies (even though the mode shapes are similar) in a SOL 103 and lowering the buckling loads (even though the mode shapes are similar) in a SOL 105. This effect increases as the RPM increases, and it becomes significant when the RPM is over 1000.

71


3.1.5.3

GL, ML P-∆ (KGA From Exact or Approximate KTA) Static Analysis

To obtain KTA, to be theoretically exact, a GNL SOL 106 (or implicit dynamic relaxation SOL 129 or explicit dynamic relaxation LS-DYNA) with prestress (as temperature loads say) and gravity must be undertaken. Alternatively, an approximation to KTA can be obtained by repetitive P-∆ static analyses with the prestress (as temperature loads say) and gravity applied. The procedure to obtain this approximate KTA will be presented. Note that the approximate KTA will be the summation of the elastic stiffness KE at the undeflected (by the prestress and gravity) state but KG at the deflected (by the prestress and gravity) state. Hence if KE changes considerably during the application of the prestress, a full SOL 106 (or implicit dynamic relaxation SOL 129 or explicit dynamic relaxation LS-DYNA), which converges to the KE and KG at the deflected (by the prestress and gravity) state should be employed. Hence for the modelling of a suspension bridge where there is a great change in geometry (known in the bridge industry as form-finding, so-called because it is necessary to find the form or shape of the catenary suspension cables), it may be prudent to employ SOL 106 (or implicit dynamic relaxation SOL 129 or explicit dynamic relaxation LS-DYNA), but for a high tension low sag cable on say a tower with prestressed cables, the repetitive P-∆ static analysis may be adequate. The repetitive P-∆ analysis basically involves a number of iterations of linear static analyses to obtain an approximate KTA. Note again that A refers to the initial undeflected (by the collapsing load) state, but deflected by the prestress and gravity. To perform the repetitive P-∆ analysis, a static analysis is performed based on KEA with temperature loads and gravity to generate forces in the structural elements, which in turn provides input for the computation of KGiAKTm where m is the iterations. Repetitive static analysis is performed with the prestress and gravity updating the stiffness matrix KEA + KGiAKTm-1 + KGiAKTm until convergence of displacements is obtained. The tangent stiffness at this stage is the approximate converged tangent stiffness matrix KTA = KEA + KGiAKT. The converged displacements represent the approximate P∆ (KGA From Approximate KTA) static response to the initial prestress loads. The converged geometric stiffness at this stage would be that based upon the approximate tangent stiffness matrix KTA, i.e. KGiAKT. Phase 1

Perform static analysis (with prestress and gravity) based on [KEA] but include the segyroa.v2001 alter prior to the Case Control Section in order to compute the geometric stiffness matrix [KGA]1 (and output into a .pch file) based on the generated element loads from the [KEA] static analysis. Phase 2

Perform static analysis (with prestress and gravity) based on [KEA] + [KGA]1 by including the k2gg = ktjj statement in the Case Control Section, the outputted .pch file which contains the ktjj matrix in the Bulk Data and the segyroa.v2001 alter prior to the Case Control Section to compute the [KGA]2 (and output into the .pch file overwriting previous data) based on the generated element loads from the [KEA] + [KGA]1 static analysis. Phase 3

Repeatedly perform the Phase 2 static analysis (with prestress and gravity) based on [KEA] + [KGA]i for i = 2 to n where n represents the number of iterations required for the change in deflections between analyses to become negligible. This would signify that the change in the [KGA] matrix become negligible and the correct [KGA] is attained. The deflections and the other responses at this stage represent the P-∆ (KGA From Approximate KTA) static response to the prestress and gravity. The stiffness of the structure is KTA. Phase 4

The P-∆ response to a general loading function can now be ascertained by performing a P-∆ static analysis with the converged tangent stiffness of the structure, KTA. The responses at this stage represent the P-∆ (KGA From Approximate KTA) response to the general loading function.

72


3.1.6

Hand Methods Verification

3.1.6.1

Static Displacements by the Unit Load Method of the Virtual Work Principle

P ∆ = f δ expresses virtual work i.e. external work = internal work P’∆ = f ’δ expresses the load method where P’ = virtual external action, specified usually as unity for the unit load method ∆ = real external kinematic, the item to be found f ’ = virtual internal action, due to the virtual external actions P’ δ = real internal kinematic, due to the real external actions on the structure 1’∆ = f1’δ expresses the unit load method 1’∆1 = f1’δ1 represents the unit load method with the real external actions also unity i.e. both the virtual external actions and real external actions are unity ∆ 1 = external real kinematic due to unit external real action = f1 ' δ 1 =

∫ (M )

 M1  ds  +  EI  R

(

 P1spring  V  k spring

1 V 

+ P1spring

∫

= M1

)

∫ (P )

 P1  P L ds  or (P1 ) V  1  +  EA  R  EA  R

1 V 

  + M 1spring  R

(

  M 1spring  V  k rotational  spring

)

   + T1spring  R

(

∫ (T )

 T1   ds  +  GK t  R

1 V

  T1spring  V  k torsional  spring

)

∫ (V )

 V1 Q  ds   GIb  R

1 V 

    R

P1sp M 1sp T1sp M1 P PL T VQ ds + P1 1 ds or P1 1 + T1 1 ds + V1 1 ds + P1sp + M 1sp + T1sp EI EA EA GK t GIb k sp k rot sp k tor sp

∫

∫

∫

The integrals can be evaluated using classical calculus integration methods, product integrals or using the numerical Simpson’s Rule I = h/3[f0+4f1+f2]. Simpson’s Rule is exact for the multiplication of continuous functions up to and including cubic variations. Non-continuous piecewise functions should be split at the discontinuities and integrated in sections.

73


74


75


3.1.6.2

BMD and SFD of Structures of Low Static Indeterminacies by Flexibility Analysis

The flexibility analysis is performed as follows (i) (ii) (iii) (iv)

(v)

(vi)

Determine the degree of static indeterminacy αs Choose αs shear force, bending moment, external force or external moment releases to form the released statically determinates structure Evaluate response of the released structure to the real external loads, m0, p0, t0 Evaluate responses of released structure (in the absence of real loads) to unit values of the releases in turn, m1, m2 … mα , p1, p2 … pα , t1, t2 … tα Note that releasing an internal bending moment or shear force constitutes the release of an internal biaction whilst the release of an external moment or force constitutes only a single action. Set up and solve the compatibility equations simultaneously f10 + X1f11 + X2f12 + … + Xα f1α = 0 f20 + X1f21 + X2f22 + … + Xα f2α = 0 ……………………………………. fα0 + X1fα1 + X2fα2 + … + Xα fαα = 0 where fij is the displacement due to virtual action i and real kinematic j. The internal bending moments, shear forces and torsional moments of the statically indeterminate structure are then given by m = m0 + X1m1 + X2m2 + … + Xαmα p = p0 + X1p1 + X2p2 + … + Xαpα t = t0 + X1t1 + X2t2 + … + Xαtα

76


77


78


79


80


81


82


83


84


85


86


87


88


89


90


91


92


93


94


95


96


97


3.1.6.3

Bending Moments, Shear Force, and Displacements of Structural Elements by the Stiffness Method

The flexural stiffness relations for a beam element gives the relationships between the actions shear force & bending moment and the kinematics displacements and rotations.

Beam With Both Ends Fixed Same End of Beam

Opposite End of Beam

Bending Moment / Rotation

4EI/L

2EI/L

Shear Force / Translation

12EI/L3

−12EI/L3

Bending Moment / Translation or Shear Force / Rotation

±6EI/L2

Beam With One End Fixed And The Other Pinned Same End of Beam



3EI/L

0


3EI/L3

−3EI/L3


±3EI/L2 but no force (hence stiffness) generated by rotation of pinned end and no moments generated at pinned end due to other kinematics

Beam With Both Ends Pinned Same End of Beam



0

0


0

0


0

The force-displacement relationship of the Timoshenko beam is as follows. For the Euler-Bernoulli beam, β is zero.

 F1   12 M   EI  6L  1  = 3  F2  L (1 + β ) − 12  M 2   6L

6L

(4 + β)L

2

− 6L

(2 − β)

  δ1  − 6L (2 − β )L   θ1    12 − 6 L  δ 2   − 6L (4 + β )L2  θ 2  − 12

6L

2 

98

β=

12EI GAL2


3.1.6.4

Bending Moments and Shear Force of Structures of Low Kinematic Indeterminacies by Moment Distribution

Fixed end forces due to distributed loading is −/+ωL2/8 and that due to a mid point load is −/+PL/8. The drop-down due to distributed loading is ωL2/8 and that due to a point load is PL/4. The distribution factors summary is as follows

Location Kinematic DOF Kinematic Fixity Pinned End Cantilever

Distribution Factor Stiffness Ratio Nothing 1 1:0

The analysis of a structure with kinematic indeterminacy αk = 1 is exact, and those with αk > 1 is iterative. The kinematic indeterminacies are reduced by (a) changing moment/rotational stiffness of pinned end beam to 3EI/L from 4EL/L, hence eliminating the pinned ended kinematic (b) employing symmetry and anti-symmetry of structure and loading as follows (i) axis of symmetry through a joint and symmetric loading φcentre = 0, hence analyze half structure with equivalent central rotational fixity (ii) axis of symmetry through a joint and anti-symmetric loading BMcenter = 0, hence analyze half structure with equivalent central pinned end (iii) axis of symmetry through a member and symmetric loading analyze half structure with the stiffness of middle member of 2EI/L (iv) axis of symmetry through a member and anti-symmetric loading analyze half structure with the stiffness of middle member of 6EI/L Hence, the analysis of pinned ended two-span continuous beams and propped cantilever is exact.

Beam and External Load Simply supported beam uniformly loaded w Simply supported beam mid-span point load P Cantilever uniformly loaded w Cantilever free-end point load P Fixed-ended beam (both sides) uniformly loaded w Fixed-ended beam (both sides) mid-span point load P Propped cantilever uniformly loaded w Propped cantilever mid-span point load P

99

Effects Mmid = wL2/8 Mmid = PL/4 Mfixed-end = wL2/2 Mfree-end = PL Mfixed-end = wL2/12 Mmid = wL2/24 Mfixed-end = PL/8 Mmid = PL/8 Mfixed-end = wL2/8 Msag = 9wL2/128 Mfixed-end = 3PL/16 Msag = 5PL/32

Bending Deflection δ = 5wL4 / (384EI) δ = PL3 / (48EI) δ = wL4 / (8EI) δ = PL3 / (3EI) δ = wL4 / (384EI) δ = PL3 / (192EI) δsag = wL4 / (185EI) δsag = 0.00932PL3/EI


100


101


102


103


104


105


106


107


108


109


110


111


112


113


114


115


116


117


118


119


120


121


122


3.1.6.5

Summary of Deflections and Effects

123


124


125


126


127


128


129


130


131


132


133


134


135


136


137


138


139


140


141


142


143


144


145


146


147


148


149


150


151


152


153


154


155


156


157


158


159


160


161


162


163


3.1.6.6 3.1.6.6.1

Member Buckling Check Using The P-∆ Method To Incorporate Imperfections, Residual Stresses ML, GL (P-∆ Based) Perry-Robertson Buckling of Column (Primary Stress is Only Axial) Elements With Imperfections and Residual Stresses

Euler buckling considers only the axial stresses with no provisions for bending stresses. Hence, it is only valid for perfectly straight columns. Perry-Robertson on the other hand includes the decrease in capacity due to initial imperfections of the column. It is based upon finding the mean axial stress that will cause the onset of yielding of extreme fibers due to the combined effects of both axial stresses and longitudinal bending stresses. Hence PerryRobertson implicitly includes yielding of the column at low slenderness ratios. It can be shown starting from the basic equation for the onset of outer fiber yielding (utilizing the amplification factor derived in Section 3.1.2, hence the reason it is called buckling by the P-∆ method)    PPR M  1   = σy + A Z  1 − PPR   PE  

i.e.

σ PR

Px 0 + Z

    1   = σy  1 − PPR  PE  

that the Perry-Robertson buckling capacity stress is

σ PR =

σ y + (1 + η )σ E 2

 σ y + (1 + η)σ E  −   − σyσE 2   2

where the Perry factor, η =

Ax 0 x 0 y x 0 y = 2 = Z r r r

The Perry factor η above is the theoretical imperfection factor which is dependent upon the initial eccentricity, x0 and also the cross sectional properties. But BS 5950-Part 1:2000 goes a step further and requires an increase in the Perry factor due to residual stresses from rolling and welding. It thus states that the Perry factor should be

η=

a (L e − L o ) 1000 ry

a = Robertson constant

The Robertson constant, a divided by 1000, i.e. a/1000 is equivalent to (x0/L)(y/r) and includes the initial imperfection, the section shape and also residual stresses. The Lo plateau is introduced so that for a very low slenderness, the strut reaches its full yield capacity. As an aside, note that although the radius of gyration of an area has no physical meaning, we can consider it to be the distance (from the reference axis) at which the entire area could be concentrated and still have the same moment of inertia as the original area. Note that σPR approaches σE for large slenderness ratios i.e. for very slender columns; This means that the sensitivity of slender columns to imperfections is less than that of stocky columns. σ cr

σ cr = σ y

σy

σ cr = σ E

σ cr = σ PR

Le = r

Le r

π2E σy

164


The capacity to buckling should be checked about both the major and minor axes. The slenderness is a function of the cross section and the boundary conditions, hence the critical buckling capacity may occur about either the major or minor axes. The critical load capacity is PPR = σ PR A

Column Buckling Check BS 5950-Part 1:2000 Allocation of strut curve = f (section type, max thickness, axis of buckling) Compressive strength, pc, smaller of pcxx = f(py,λxx) and pcyy = f(py,λyy) (N/mm2)

cl. 4.7.4 Table 23 Table 24

Slenderness, λxx = LExx / rxx and λyy = LEyy / ryy Effective length, LExx and LEyy

Table 22

Ensure F/(Apc) < 1 for Class 1, 2 and 3 sections

cl. 4.7.4

Note that for welded I, H or box sections, pc should be obtained from Table 24 or calculated using a py value lessened by 20 N/mm2. A fundamental parameter is the effective length, LE.

165


Another method used to determine LE in buildings given in BS 5950-Part 1:2000 is based on the adjacent member stiffnesses to determine coefficient k1 and k2 from which design charts are used to determine LE for sway and nonsway frames.

Non-Sway

Sway

166


The choice of strut curve is defined by Table 23 as follows.

The pc of Table 24 can be calculated as

where

and the Perry factor, η in which the limiting slenderness λ0 is and the Robertson constant, a is defined as follows

167


168


On top of the Perry-Robertson flexural buckling, columns are also subject to torsional buckling and flexuraltorsional buckling. These occur when the ratio of torsional to flexural stiffness is very much reduced.

169


3.1.6.6.2

ML, GL (P-∆ Based) Secant Buckling of Column (Primary Stress is Axial) Elements With Eccentric Loading, Initial Imperfections and Residual Stresses

The Secant buckling stress for an eccentrically (with eccentricity e) loaded column is as follows. It is based upon finding the mean axial stress that will cause the onset of yielding of extreme fibers due to the combined effects of both axial stresses and longitudinal bending stresses, the latter of which is primarily a result of the eccentricity of the axial load. The initial imperfections and residual stresses can also be added to the loading eccentricity, e for an equivalent eccentricity, e. σy σ SECANT = L σ SECANT  ec 1 + 2 sec  e  2r  E r   The equation is an implicit formula, and hence iteration is required to solve for σSECANT. Note that the radius of gyration, r is the minor axis radius of gyration. Also, c denotes the distance from the neutral axis to the extreme fibre on the concave or compression side of the bent column. The term ec/r2 is called the eccentric ratio, a value which is often calibrated to physical tests. In fact, it is the same as the Perry factor, η had there been no eccentricity of the loading. Typical conventional design of structural steel columns employs a value of 0.25 for ec/r2.

170


3.1.6.6.3

ML, GL (P-∆ Based) Lateral-Torsional Buckling of Beam (Primary Stress is Only Bending) Elements With Imperfections and Residual Stresses

A critical parameter is the effective length, LE and is defined in clauses cl. 4.3.5.1 to cl. 4.3.5.5 for

simple beams without intermediate lateral restraints (Table 13), simple beams with intermediate lateral restraints (1.0LLT normal loads or 1.2LLT destabilizing loads), beams with double curvature bending, cantilever beams without intermediate lateral restraints (Table 14), cantilever beams with intermediate lateral restraints (1.0L normal loads or Table 14 destabilizing loads). Note that LLT is the segment length between restraints, and the span length is L. Note that the destabilizing loading condition should be taken where a load is applied to the top flange of a beam or a cantilever, and both the load and the flange are free to deflect laterally (and possibly rotationally also) relative to the centroid of the cross-section.

Lateral Torsional Buckling Moment Capacity, Mb / mLT BS 5950-Part 1:2000 Critical slenderness about minor axis λyy = LEy/ry Effective length, LEy

cl.4.3 cl. 4.3.5.1 to cl 4.3.5.5

Radius of gyration about the minor axis, ry

Effective critical axis slenderness λLT = uvλ(βW)0.5 Buckling parameter, u For rolled equal flange I-, H- or channel section, u = 0.9 conservatively Torsional index, x For rolled equal flange I-, H- or channel section, x = D/T conservatively Slenderness factor, v = f(λ/x,flange ratio η) For equal flange I-, H- or channel v = 1/(1+0.05(λ/x)2)1/4 βW = 1.0 for Class 1 plastic and Class 2 compact sections

cl. 4.3.6.8 cl. 4.3.6.8 cl. 4.3.6.7 Table 19 cl. 4.3.6.9

Lateral torsional buckling moment capacity, Mb/m Buckling resistance moment, Mb = pbSx for Class 1 and Class 2 sections Buckling resistance moment, Mb = pbZx for Class 3 sections Buckling resistance moment, Mb = pbZeff for Class 4 sections

cl. 4.3.6.4 cl. 4.3.6.5 Table 16 or Table 17

Bending strength, pb = f(py,λLT)

cl. 4.3.6.6 Table 18

Equivalent uniform moment factor, mLT

Ensure LTB moment capacity Mb/mLT > applied design moment Md Lateral torsional buckling cannot occur in beams loaded in their weaker principal plane; under the action of increasing load they will collapse simply by plastic action and excessive in-plane deformation. Hence, the check need only be made for bending about the major axis. Lateral torsional buckling cannot occur for sections which are double symmetric such as a SHS, this being accounted for by the fact that λLT becomes zero when Ixx = Iyy. The equivalent uniform moment factor, mLT is used when the bending moment is not uniform across the length of the beam. A value of 1.0 is obviously conservative. For the destabilizing loading condition mLT should be taken as 1.0. The LTB bending resistance given by Table 16 or Table 17 is derived from

171


where

where the Perry factor ηLT

and where the Robertson constant aLT should be taken as 7.0 and the limiting equivalent slenderness, λL0 is

Restraints may be deemed to provide adequate stiffness and strength if capable of resisting a lateral force of at least 2.5% of the maximum factored force in the compression flange.

172


173


174


3.1.6.6.4

ML, GL (P-∆ Based) Buckling of Beam-Column Elements (Primary Stress is Axial and Bending) With Imperfections and Residual Stresses

Simplified Approach (cl. 4.8.3.3.1) For Perry-Robertson flexural buckling about the major or minor axes with additional primary moments about the major and minor axes, the following expression must be satisfied Although unconservatively no amplification of major axis moment considered, conservatively the minor axis elastic capacity is used. Note that Pc is the Perry-Robertson flexural buckling capacity and is the smaller of Pcx and Pcy. The major axis flexural buckling factor, mx and the minor axis flexural buckling factor, my are obtained from Table 26 (cl. 4.8.3.3.4). For lateral torsional buckling with Perry-Robertson flexural buckling about minor axis and additional primary moment about minor axis, the following expression must also be satisfied. Although unconservatively no amplification of minor axis moment considered, conservatively the minor axis elastic capacity is used. Note that Pcy is the minor axis Perry-Robertson flexural buckling capacity. MLT is the applied major axis moment. My is the applied minor axis moment. Mb / mLT is the lateral torsional buckling capacity.

More Exact Approach for I- or H- Sections with Equal Flanges (cl. 4.8.3.3.2) For Perry-Robertson flexural buckling about the major with additional primary moments about the major or minor axes, the following expression must be satisfied

where myx is obtained from Table 26 (cl. 4.8.3.3.4). The major axis flexural buckling factor, mx is also obtained from Table 26 (cl. 4.8.3.3.4). Note that Pcx is the major axis Perry-Robertson flexural buckling capacity. Mx and My are the major and minor axes applied moments. Mcx and Mcy are the major and minor axes plastic moment capacities. For lateral torsional buckling (of course about minor axis) with Perry-Robertson flexural buckling about minor axis and additional primary moment about minor axis, the following expression must also be satisfied.

For an interactive buckling, the following expression must also be satisfied.

Similar more exact equations exist for CHS, RHS and box sections with equal flanges in cl. 4.8.3.3.3.

175


176


3.1.6.7

Overall Portal Frame and Multi-Storey Building P-∆ Analysis Using The Amplified Sway Method

Sufficient lateral stability must be provided to prevent instability. Sufficient strength must be provided to take the increased forces (P-∆ effects) as a result of the slenderness. To investigate the susceptibility of a structure to P-∆ effects, the elastic buckling load factor is calculated. Methods based on BS 5950-Part 1:2000 for calculating λcr is given in Section 3.2.5.2.2. Then assuming 4 < λcr <10, the P-∆ effects should be taken into account for the real horizontal loads (wind) according to the amplified sway method. Had λcr been greater than 10, then the building is considered non-sway and amplification effects, m on lateral forces need not be considered. For portal frames, if under the Notional Horizontal Forces (NHF) of the gravity load combination, the horizontal deflections at the tops of the column are less than height/1000, P-∆ effects need not be considered. Had λcr been less than 4, then a full nonlinear static analysis must be undertaken to account for the P-∆ effect. The amplified sway factor for the real horizontal loads (wind) (in perfect accordance with theory presented in Section 3.1.2) is (cl. 2.4.2.7) λ cr m= λ cr − 1 For clad structures with the stiffening effect of masonry infill wall panels or diaphragms of profiled steel sheeting the amplified sway factor is decreased to λ cr m= but m > 1.0 1.15λ cr − 1.5 The ULS load combinations are presented in Section 8.2.3. Note the load case corresponding to the NHF includes the factored dead and live load.

177


3.2

GL, ML Buckling Analysis by The Implicit Linearized Eigenvalue Analysis

3.2.1

Linearization of Tangent Stiffness Matrix and Formulating The Linear Eigenvalue Problem λ ML, GL Static Analysis ML, GL Buckling Analysis λECR ML, GL P-∆ Static Analysis ML, GNL Static and Buckling Analysis (Tracing Equilibrium Path or Implicit or Explicit Time Integration with Dynamic Relaxation) MNL, GL Plastic Collapse Analysis λP



This section describes a simple and practical method of allowing for the effects of overall buckling of the structure. While the method can be applied to the buckling of single members, this is more easily dealt with using conventional codified methods. Where conventional codified methods falls short, is when the boundary conditions of the structural members (which determines the all important buckling effective length) is not intuitive. Linear elastic buckling analysis is the prediction of the critical loads (and their associated buckling mode shapes) when the structure is at the point of elastic instability. This instability occurs when the tangent stiffness matrix becomes singular as a result of the increase in the negative stiffness contribution of the geometric (differential) stiffness. At collapse, the structure has buckled (experienced elastic instability) but has no fully plastic hinges i.e. no considerations of material nonlinearity have been taken into account. Hence this method of analysis is only valid if firstly, the structure remains materially linear elastic throughout until the application of the critical load causes an elastic instability. Secondly, it is a geometrically linear method of analysis. Hence the deflections must be small enough for the stiffnesses to be based upon the initial undeflected (by the collapsing load factor) geometry. Let us denote the initial undeflected (by the collapsing load factor) configuration by A. In the (KGA From KEA) elastic buckling analysis, at collapse, the elastic stiffness matrix at the initial undeflected (by the collapsing load factor) configuration is balanced by the geometric (differential) stiffness due to the load factor.

[[K

A E ]+

]

λ[ K GAKE ] {φ} = {0}

AKE

KG represents the geometric stiffness matrix which was calculated based on the small displacements obtained by solving the system (with the collapsing load) with stiffness KEA. Hence, a static analysis is first performed (a first pass) based on KEA with an applied external load (which is a fraction of the critical buckling load so that the buckling load factor will be more than 1) to generate forces in the structural elements, which in turn provides input for the computation of KGAKE. Then, a buckling analysis is performed effectively finding the instances when factored by λ, KGAKE balances KEA. Hence, since both the elastic stiffness matrix KEA and the geometric stiffness matrix KGAKE are based upon the initial undeflected (by the collapsing load factor) configuration A, the method is only valid if deflections are small enough for there to be negligible change in KEA and the geometric stiffness matrix varies linearly with the load factor such that it can be expressed as λKGAKE until elastic instability has been attained. The inherent assumption that the geometric stiffness matrix varies linearly with the load factor λKGAKE enables any external load to be applied in the first pass since KGAKE will be scaled accordingly. Hence, any initial load (less than the collapse load so that λ < 1) may be applied and the corresponding load factor λ will be obtained such that the collapse load λPinitial or rather expressed as λPnA will be the same. The value λ are the scale

178


factor by which the applied load PnA is multiplied to produce the critical buckling load Pcr. The magnitude of the applied load PnA is arbitrary for arriving at the correct Pcr. As an example, if PnA is increased by a factor of 10, then the calculated value of λ is reduced by a factor of 10; in other words, their resulting product Pcr remains the same. This is because the differential stiffness of the finite elements are linear functions of the axial load Fx and the geometry l of the element (as shown below for the CBAR element) and for linear analyses, the axial load increases linearly with the applied loads PnA.

Clearly, assuming that deflections are indeed small, the method is only valid for the first buckling mode as subsequent deflections will certainly be too large. To illustrate the assumption, this linearized buckling analysis basically traces the following equilibrium path. λ ML, GL Static Analysis ML, GL (KGA From KEA) Buckling Analysis λECR

KE

ML, GNL Static and Buckling Analysis (Tracing Equilibrium Path or Implicit or Explicit Time Integration with Dynamic Relaxation)

A

[ ] {P }

∆{U} = λ K AE

−1

A n

U

That is to say, the structure follows the equilibrium path governed by the constant stiffness KEA until suddenly it loses all its stiffness (in a direction dissimilar to that of the critical load) and buckles when λKGAKE matches KEA. This is valid if KEA is assumed not to vary with the {U} and if the component forces {f} are approximately linear in terms of the load factor λ such that the geometric stiffness matrix varies linearly with the load factor allowing it to be expressed as λKGAKE until elastic instability has been attained, both of which are quite valid as long as the tangential increment of displacement due to λ is small. This can be estimated from

[ ] {P }

∆{U} = λ K AE

−1

Hence, the forces at linear buckling are the load factor times the linear static displacement.

A n

where ∆{U} is the tangential increment of displacement due to λ. From the expression above, clearly the same elastic buckling displacement (and force) response will be obtained irrespective of the initial loads applied as λ will be obtained to scale the responses accordingly. Hence, in this approach, the response at buckling is insensitive to the initial loads applied. Conversely, calculating the displacement response from a P-∆ static analysis, we will find that the initial loads applied do affect the response at buckling. The P-∆ response is obtained from

{U m } = [K AE

A + K Gm

] {{P −1

m

} + {Fixed End Forces}m

[

]

}

A − K Gm {U 0 }

179


where KGA which depends on the initial loads is obtained from a first pass

{U m } = [K AE ] {{Pm } + {Fixed End Forces }m } −1

The slightly nonlinear P-∆ path traced is shown below. λ

ML, GL Static Analysis ML, GL Buckling Analysis λECR ML, GL P-∆ ∆ Static Analysis ML, GNL Static and Buckling Analysis (Tracing Equilibrium Path or Implicit or Explicit Time Integration with Dynamic Relaxation) MNL, GL Plastic Collapse Analysis λP



Of course, P-∆ response calculations become inaccurate when the initial load {Pm} applied is very high such that had a linearized buckling analysis been performed, the elastic buckling load factor λ would be less than 4. Both the buckling load factor scaled response and the P-∆ response is not ideal. In reality of course, the gradual application of the load would cause a gradual reduction of stiffness (as the differential stiffness gradually becomes more negative) until buckling occurs as depicted on the smoothed curve above. This path can be traced by performing a nonlinear static and buckling analysis (MSC.NASTRAN SOL 106) and is the recommended approach to determining the response (displacement and element forces) at buckling. The above (KGA From KEA) may prove inadequate in many instances such as when there is prestress in the elements even before the application of the collapsing load factor. In this case, the (KGA From KTA) elastic buckling analysis is performed where at collapse, the tangent stiffness matrix at the initial undeflected (by the collapsing load factor, but includes the stiffness contribution of prestressed members) stage A configuration is balanced by the geometric (differential) stiffness due to the load factor.

[[K

A T ]+

]

AKT λ[ K Gn ] {φ} = {0}

AKT

KGn represents the geometric stiffness matrix which was calculated based on the small displacements obtained by solving the system with a linear static analysis (with the collapsing load) with stiffness KTA. To obtain KTA, to be theoretically exact, a GNL SOL 106 (or implicit dynamic relaxation SOL 129 or explicit dynamic relaxation LSDYNA) with prestress (as temperature loads say) and gravity must be undertaken. Alternatively, an approximation to KTA can be obtained by repetitive P-∆ static analyses with the prestress (as temperature loads say) and gravity applied. The procedure to obtain this approximate KTA will be presented. Note that the approximate KTA will be the summation of the elastic stiffness KE at the undeflected (by the prestress and gravity) state but KG at the deflected (by the prestress and gravity) state. Hence if KE changes considerably during the application of the prestress and gravity, a full SOL 106 (or implicit dynamic relaxation SOL 129 or explicit dynamic relaxation LS-DYNA), which converges to the KE and KG at the deflected (by the prestress and gravity) state should be employed. Hence for the modelling of a suspension bridge where there is a great change in geometry, it may be prudent to employ SOL 106 (or implicit dynamic relaxation SOL 129 or explicit dynamic relaxation LS-DYNA), but for a high tension low sag cable on say a tower with prestressed cables, the repetitive P-∆ static analysis may be adequate. The repetitive P-∆ analysis basically involves a number of iterations of linear static analyses to obtain an approximate KTA. Note again that A refers to the initial undeflected (by the collapsing load) state, but deflected by the prestress and gravity. To perform the repetitive P-∆ analysis, a static analysis is performed based on KEA with temperature loads and gravity

180


to generate forces in the structural elements, which in turn provides input for the computation of KGiAKTm where m is the iterations. Repetitive static analysis is performed with the prestress and gravity updating the stiffness matrix KEA + KGiAKTm-1 + KGiAKTm until convergence of displacements is obtained. The tangent stiffness at this stage is the approximate converged tangent stiffness matrix KTA = KEA + KGiAKT. The converged displacements represent the approximate P-∆ (KGA From Approximate KTA) static response to the initial prestress loads and gravity. The converged geometric stiffness at this stage would be that based upon the approximate tangent stiffness matrix KTA, i.e. KGiAKT. Irrespective of the method of obtaining KTA, whether by SOL 106 (or implicit dynamic relaxation SOL 129 or explicit dynamic relaxation LS-DYNA) or repetitive P-∆, another static analysis is performed on KTA, this time with the collapsing applied external loads (which is a fraction of the critical buckling load so that the buckling load factor will be more than 1). This generates KGnAKT. Then, a buckling analysis is performed, effectively finding the instances when factored by λ, KGnAKT balances KTA. Hence, since both the tangent stiffness matrix KTA and the geometric stiffness matrix KGnAKT are based upon the initial undeflected (by the collapsing load factor) configuration A, the method is only valid if deflections are small enough for there to be negligible change in KTA and the geometric stiffness matrix varies linearly with the load factor such that it can be expressed as λKGnAKT until elastic instability has been attained. The inherent assumption that the geometric stiffness matrix varies linearly with the load factor λKGnAKT enables any external load to be applied in the first pass since KGnAKT will be scaled accordingly. However, in any FE model, even an extremely linear one, the geometric stiffness matrix does not actually vary perfectly linear with the load factor, hence choosing a different external load value as a first pass will result in minor discrepancies in the load factor. Clearly, assuming that deflections are indeed small, the method is only valid for the first buckling mode as subsequent deflections will certainly be too large. To illustrate the assumption, this linearized buckling analysis basically traces the following equilibrium path. λ ML, GL Static Analysis ML, GL (KGA From KTA) Buckling Analysis λECR

KT

A

ML, GNL Static and Buckling Analysis (Tracing Equilibrium Path or Implicit or Explicit Time Integration with Dynamic Relaxation)

U

That is to say, the structure follows the equilibrium path governed by the constant stiffness KTA until suddenly it loses all its stiffness (in a direction dissimilar to that of the critical load) and buckles when λKGnAKT matches KTA. This is valid if KTA is assumed not to vary with the {U} and if the component forces {f}n are approximately linear in terms of the load factor λ such that the geometric stiffness matrix varies linearly with the load factor allowing it to be expressed as λKGnAKT until elastic instability has been attained, both of which are quite valid as long as the tangential increment of displacement due to λ is small. This can be estimated from

[ ] {P }

∆{U} = λ K TA

−1

A n

where ∆{U} is the tangential increment of displacement due to λ. In reality of course, the gradual application of the load would cause a gradual reduction of stiffness (as the differential stiffness gradually becomes more negative) until buckling occurs as depicted on the smoothed curve above. This path can be traced by performing a nonlinear static and buckling analysis (MSC.NASTRAN SOL 106). Buckling analyses based on KTA is used in instances where there is prestressing and gravity before the application of the critical buckling loads, for instance in the buckling of suspension bridge piers or cable prestressed towers. A static solution based upon KTA (incorporating the prestress and gravity) which is obtained exactly by SOL 106

181


(or implicit dynamic relaxation SOL 129 or explicit dynamic relaxation) or approximately by repetitive P-∆ analysis (the latter may be valid for low sag high tension cable problems where KE does not change much due to the prestress and gravity) must be first obtained. Then, the buckling load is applied to generate the geometric stiffness matrix (for that buckling load) and an eigenvalue analysis is performed. The nonlinear (in that it is dependent upon {U}) tangent stiffness matrix is restated as follows.

[K T ] = [K E ] + [K G ] where [K E ] = [T ]T [[k E ]][T ] [k E ] = ∫ [B]T [D][B]dΩ for which Ω

 ∂2 d



[K G ] = [T]T [[k G ]][T] + 

and

 ∂{U}∂ U

 ∂2 ε

[k G ] = ∫ 

for which and

 ∂ {d}∂ d {σ}n = [ D ][ B ]{d}

and

{f } =

{f } 



 ∂ 2 Wi   ∂ 2 Wn    − λ  ∂ {d}∂ d   ∂ {d}∂ d 

{{σ}n + {σ}i − [ D ]{ε}i }dΩ −  

Ω

[∫ [B] [D ][ B]dΩ ]{d} + {∫ [B] {σ} dΩ}− {∫ [B] [D ]{ε} dΩ}− {∫ [ N ] {b}dΩ} T

T

Ω

Τ

T

i

Ω

i

Ω

Ω

As stated, we have omitted the second order variation of work due to the external nodal loadings {P} from the above tangent stiffness matrix expression, i.e.

 ∂2W −  ∂{U}∂ U

  ∂{P}   = −    ∂ U 

as

 ∂W  {P} =    ∂{U}

This is because, as mentioned, the externally applied loads at the nodes are in commercial codes always workconjugate with the nodal DOFs {U}, failing which the above term must be incorporated. The second order variation of work due to loads applied on the finite elements is obviously still taken into account. [KT] is inherently nonlinearly dependent upon λ and {U}. The buckling problem can be expressed as a linear eigenvalue problem if [KT] is assumed not to vary with the {U} and if the component forces {f} are approximately linear in terms of the load factor λ. The objective is to linearize the eigenvalue problem around the initial equilibrium state A. The first order change in [KT] for state A

[K ] = [K ] + ∆[K ] = [K ] + ∆[K ] + ∆[K ] ∆ [K ] = ∆[T ] [ k ][T ] + [T ] [ k ]∆[T ] T

A T

A T

T

T

E

 ∂2 d ∆ KG =   ∂{U}∂ U 

[ ]

E

A E

A

A

G

A T

A E

  ∂2W n ∆{f } − ∆λ    ∂{U}∂ U  

A

  ∂2 d  + ∆   ∂{U}∂ U  

A



  ∂ W  {f } − ∆  ∂{U∂ }W  − λ ∆  ∂{d}∂ d ∂ U 2

A

2

A

i







n





Although the above can be used directly for formulating a linear eigenvalue problem, the influence of a change of geometry on [KT] is normally ignored, and hence ∆[KE] and the last 3 components of ∆[KG] are ignored. The linearized buckling (eigenvalue) problem is thus expressed as

[K T ]{φ} = {0}

([K ] + λ[K ]){φ} = {0} A T

A Gn

182


The nontrivial solution is obtained by solving for the eigenvalue λ in the expression DET ([K T ]) = 0, the corresponding {φ} being the eigenvector or the buckling mode shape

([ ] [ ]) [ ] = [K ] + [K ]

A =0 DET K TA + λ K Gn

K TA

A E

A G

[ ] [ ][T ] + [T ]

=T

[K ] A Gn

where

A T

k AE

 ∂2 ε =  ∂{d}∂ d 

A

 ∂2 ε  ∂{d}∂ d 

A

A T

A

  2 ∂ Wn {σ}An  −    ∂{d}∂ d  

{{ } σ An

A

  ∂2 d +   ∂{U}∂ U  

{f }= {∫ [B] {σ} dΩ}− {∫ [B] [D]{ε} dΩ} {f }= [∫ [B ] [D ][B ]dΩ ]{d }− {∫ [ N] {b} A i A n

T

− [ D]{ε}iA A

}

∂ 2 Wi − ∂{d}∂ d

A

 ∂2 d  TA +    ∂{U}∂ U  

[ ]

A



{f } A i





{f } A n



T

i

Ω

+ {σ}iA

A T

i

Ω

A

Ω

A

A n

T

Ω

n

dΩ

}

The displacements are estimated from the following equation

[ ] {P }

∆{U} = λ K TA

−1

A n

where ∆{U} is the tangential increment of displacement due to λ. The physical meaning of the [KTA] matrix is that it represents the tangent stiffness matrix at the initial undeflected configuration with the effect of the prestress and the initial second order work variation included. In the linearized buckling analysis, a load factor is found which causes the tangent stiffness to become zero by a term which multiplies this load factor to the nominal part of the geometric (or differential) stiffness based on the initial undeflected configuration. The nominal part refers to the additional element force {fn} and additional work Wn terms, not the prestress {fi}. Hence, it is assumed that in the application of the load factor that both the nominal internal forces {fnA} and the nominal second order work term vary linearly with the load factor. These factored nominal internal force and factored nominal second order work terms are based on values at the initial state A. Also it is assumed that the transformation matrix [T] is constant at [TA]. Thus it can be concluded that the linearized buckling analysis is only valid when the deflections {U} are small i.e. to predict buckling along the trivial fundamental path or along a path close to the trivial path. A buckling point in the response of a discrete structural system is either a bifurcation point or a limit point. Accordingly, it corresponds to an equilibrium state for which the tangent stiffness matrix [KT] becomes singular, indicating the presence of an infinitesimally adjacent equilibrium state at the same level of loading. Linearized buckling analysis is based on the initial undeflected geometry, i.e. (A) = initial state to determine [KTA]. [KTA] is thus the tangential value of [KT] at the initial undeflected shape (A). There is no point in choosing another state (A) to find [KTA], as we then might as well perform nonlinear buckling analysis. Linear buckling analysis tends to provide good approximations to the critical load when the critical point is a bifurcation point. But linear buckling analysis can overestimate the critical load when the critical point is a limit point and if the buckling occurs at significant incremental deflection ∆{U} from state (A) as the change in [KT] due to the change in {U} is ignored. This value of ∆{U} is estimated using the equation stated above in order to make a judgment. Higher critical modes in linear buckling analysis are inaccurate if the first mode is a limit point due to subsequent larger deflections. Hence, linear buckling analysis is most suitable for detecting bifurcation points along trivial (or almost trivial) fundamental paths, in which case state (A) can be the initial state, and for detecting critical points which are close to the known equilibrium state (A).

183


3.2.2

Problem Reduction and Trial Modes in Linear Buckling Analysis

The number of degrees of freedom n of the linear eigenvalue problem can be reduced to m as an approximation. The linear eigenvalue problem of size n is expressed as

([K ] + ∆λ[K ]){Φ} = {0} A T

A Gn

for which the exact eigenvalue ∆λ is obtained from

([ ]

[ ])

A det K TA + ∆λ K Gn =0

and{Φ} being the corresponding buckling modes shape or eigenvector

However, an approximate solution is obtained by approximating the exact buckling mode {Φ} as a linear combination of m pre - defined modes in

[Φ t ] = [{Φ t1 } + {Φ t2 } + {Φ t3 } + ...{Φ tm }] using m unknown modal parameters {φ}, m < n {Φ} = [Φ t ]{φ}

Hence,

([K ] + ∆λ[K ])[Φ ]{φ} = {0} A T

A Gn

t

Pr emultiplying by [Φ t ] , the reduced linear eigenvalue problem of size m (m < n) is expressed as T

([k ] + ∆λ[k ]){φ} = {0} A T

A Gn

[k ] = [Φ ] [K ][Φ ] T

A T

where

t

A T

t

and

[k ] = [Φ ] [K ][Φ ] T

A Gn

t

A Gn

t

for which the approximate eigenvalue ∆λ is obtained from

([ ]

[ ])

A det k TA + ∆λ k Gn = 0 and

{φ} being the corresponding buckling modes shape or eigenvector

Naturally, the solution would be exact in this m size eigenvalue problem if the exact mode shape can be modelled by [Φ t ]. This can be done if m = n, i.e. if the number of independent modes of deformation equal the number of degrees of freedom. This would be equivalent to solving the original eigenvalue problem. In the special case that the trial mode is to be approximated straight away such that the trial mode matrix [Φ t ] reduces to a single column vector {Φ t }, then

{Φ} = {Φ t }{φ}

for which the approximate eigenvalue ∆λ is obtained from ∆λ = −

[ ] [ ]

k TA {Φ t }T KTA {Φ t } = − A A k Gn {Φ t }T K Gn {Φ t }

and {Φ t } being the corresponding buckling modes shape or eigenvector

[ ] {P }

A good approximate mode shape for uniform shear frames based on Rayleigh's is {Φ t } = K TA where {Pn } is the vertical loads applied horizontally.

−1

n

Naturally, the solution would be exact if {Φ t } is the exact mode shape. This is ensured if

[K ]{Φ } = λ[K ]{Φ } A T

t

A Gn

t

i.e.

[K ]{Φ } α [K ]{Φ } A T

t

A Gn

t

The trial mode matrix [Φt] for the problem reduction in linear buckling analysis is a multi modal matrix. The trial mode method assumes just one mode shape {Φt} whilst the problem reduction method assumes a linear combination of mode shapes, [Φt] = [{Φt1}+{Φt2}+{Φt3}+…+{Φtm}]. Hence the problem reduction method is more accurate evidently. Hence, the problem reduction method will yield a lower estimate of ∆λ than the trial mode shape method. The nonlinear eigenvalue problem will of course yield the lowest exact value of ∆λ.

184


3.2.3

Concepts of Linearized (KGA From KEA) Buckling Analysis

The concept of GL, ML buckling analysis will be illustrated for a simple system.

Let us assume that deflections are small (hence geometrically linear analysis) hence the rotation of the column segments can be described and any change in height can be neglected. Lateral equilibrium at the central pin shows that

Rearranging so that we have the form Stiffness x Displacement = Applied Force, we get

Geometric Stiffness 2N/L

and hence the deflection

We can see that the effect of the force N acting on this system can be seen as being like an additional stiffness term 2N/L, i.e. the geometric (aka differential) stiffness. The effect of the axial force is equivalent to an additional stiffness of value 2N / L acting laterally at the pin location. If the force is tensile (i.e. positive) then the geometric stiffness will act to increase the overall stiffness of the system. On the other hand, if it is compressive then the term will be negative and the system stiffness will decrease. Consider the condition at which the axial compression in our simple pin jointed system is so great that the lateral stiffness of the system is zero. i.e. At this critical load, buckling occurs. And the critical linear elastic buckling load factor λcr of the system is

It cannot be emphasized enough that, the buckling load factor is independent of the initial lateral imperfections, the lateral load and material strength. This linear buckling critical load factor is independent of the applied lateral force F and the initial lateral imperfection. Of course, the amplified displacement response is dependent upon F and the initial imperfection. The buckling factor is also independent of the material strength as it depends on the stiffness instead.

185


3.2.4 3.2.4.1

MSC.NASTRAN Decks GL, ML (KGA From KEA) Buckling Analysis

$ EXECUTIVE CONTROL SECTION SOL 105 $ CASE CONTROL SECTION DISPLACEMENT() = ALL/ $ Plots the buckled shapes SPCFORCES() = ALL/ OLOAD() = ALL/ ELSTRESS() = ALL/ ELFORCE() = ALL/ STRAIN() = ALL/ ESE() = ALL/ $ SUBCASE 1 LABEL = Static Load Case With Buckling Load LOAD = < ID of FORCEi, MOMENTi, PLOADi, GRAV, LOAD, SPCD Cards in Bulk Data > TEMP(LOAD) = < ID of TEMP, TEMPRB, TEMPP1 Cards in Bulk Data > DEFORM = < ID of DEFORM Cards in Bulk Data > SPC = < ID of SPC Cards in Bulk Data > $ SUBCASE 2 LABEL = Buckling Case STATSUB(BUCKLING) = < Static Subcase Number > SPC = < ID of SPC Cards in Bulk Data > METHOD = < ID in EIGRL or EIGB >

For medium to large models, the Lanczos method is the recommended eigenvalue extraction method. Furthermore, the Lanczos method takes full advantage of sparse matrix methods that can substantially increase computational speed and reduce disk space usage. For overall robustness, the Lanczos method is the recommended method. $ BULK DATA EIGRL

ID

Lower Eigenvalue

Upper Eigenvalue

Number of Roots

Unlike dynamic modal analysis, linear buckling analysis produces eigenvalues that can be either positive or negative. Note that these negative roots are legitimate both from a physical and a mathematical standpoint. In general, this situation only occurs if the applied buckling load is in the opposite direction of the buckling load, that is to say a buckled shape with the same magnitude of eigenvalue can be produced if the applied loading was reversed in direction. Hence, if on the EIGRL card, only the upper eigenvalue range is specified, NASTRAN will attempt to extract all eigenvectors below that value, including all the negative eigenvalues. Thus if we are only interested in the fundamental mode, it is necessary to also specify the number of roots. Buckling load factor, λ

The enhanced inverse power method (SINV) can be a good choice if the model is too large to fit into memory, only a few modes are needed, and you have a reasonable idea of your eigenvalue range of interest. It is useful for models

186


in which only the lowest few modes are desired. This method is also useful as a backup method to verify the accuracy of other methods. $ BULK DATA EIGB

ID

SINV

Lower Eigenvalue

Upper Frequency

At least two subcases are necessary, the first being the static subcase that is used in the second subcase to generate the differential stiffness matrix from the internal element loads and then solve the eigenvalue problem. The differential stiffness is supported by CONROD, CROD, CTUBE, CBAR (for both Euler and lateral torsional buckling), CBEAM, CBEND, CQUAD4, CQUAD8, CTRIA3, CTRIA6, CSHEAR, CHEXA, CPENTA and CTETRA. The contribution to the differential stiffness from the follower force effect is not included. Offsets should not be used in beam, plate, or shell elements for buckling analysis. For 3-D buckling problems, the use of PARAM, K6ROT is recommended for CQUAD4 and CTRIA3 elements. A value of 100 is recommended. Note that each subcase may have a different boundary condition. Although the element stresses, forces and strains for each buckled mode may be output, it is meaningless as they are based upon the eigenvectors that have been scaled arbitrarily. These values DO NOT INDICATE RESPONSE. To obtain the response (displacement and element forces) at buckling, the response from a linear static analysis of the initial applied loads, and scaled by the critical load factor can be used.

[ ] {P }

∆{U} = λ K AE

−1

A n

Of course though, the element strain energy density distribution (ESE request), although have likewise meaningless magnitudes (again due to arbitrary scaling of eigenvectors), is an important design tool which shows elements which work the most in causing that buckled mode shape. Stiffening elements with a high ESE would increase the buckling load factor. The number of buckled modes obtained will be limited to the number of DOFs in the finite element model. The mesh should be fine enough to represent the buckled shape. CBAR elements have cubic polynomial transverse interpolation functions (shape functions). But unlike in a static analysis where the cubic deflection over a beam element can be mapped, in a buckling analysis the deflected shape is provided only by the deflections at the nodes. Hence the beam element must be refined. Also note that the buckled mode shape of a beam member is not cubic polynomial anyway. One dimensional elements such as CBAR elements (in a fine mesh as they may be) do not model the local buckling of members. The local buckling of a tube or pipe (i.e. the crippling of the thin wall) in compression must be modeled with a fine mesh of shells. A coarse mesh may predict an unconservative larger fundamental buckling load factor as the local mode cannot be captured. It is thus important to anticipate the buckling mode, or alternatively, continuous refinement be made. Buckling is a state of loss of stiffness, an unstable state, i.e. failure. If the local crippling buckling mode is more critical than the overall beam buckling mode, it is imperative that shell elements are used as line elements will give an unconservative result. Buckling generally requires a fine mesh. If the buckled shape is jagged, it is a clear indication that the mesh is not fine enough. There must be several elements per wavelength, usually 4 (or 8, 16, 32 etc…other numbers even 5 tend to be inferior) elements per half sine wavelength. Local buckling can also be checked using hand calculations based upon the physical boundary conditions and thickness on a relevant panel to estimate the buckling stress and comparison with the stress from a linear static SOL 101 analysis to evaluate if the component would buckle under that load. Linear buckling analysis assumed the deflections to be small and the elements stresses elastic. For structures that exhibit nonlinear material or large deflection deformations, the linear buckling load obtained from Solution 105 may be different than the actual buckling load. For structures with significant nonlinearities, it is recommended that a nonlinear buckling analysis using SOL 106 be performed.

187


The preliminary scheme stage buckling analysis of the Centre Pompidou, Metz timber roof is presented.

Centre Pompidou Timber Roof Scheme Design Linear Buckling Analysis Linearized Buckling Due To Self-Weight (Applied Vertical Resultant 9547kN) The applied load consists of timber planks (6097kN), intermediate packs (1039kN) and roof covering (2411kN). The linearized buckling problem is

[[K

A E ]+

]

λ[ K GAKE ] {φ} = {0}

The instantaneous and geometric stiffnesses are based on the unfactored 5th percentile stiffness values (E = 12GPa; G = 0.4GPa) for the timber material, hence conservative as far as buckling analysis is concerned. The geometric stiffness is a function of the internal forces. For example, for a straight column subject to axial compression F, the geometric stiffness is simply F/L. The critical load case which causes the greatest compression and hence the greatest geometric stiffness is sought. The lowest buckled mode shape (which could be replicated in reality) due to self-weight is presented. The load factor is 16.9. Note that there was another mode with a load factor of –14.75, this indicating an upward gravity, which is implausible, hence ignored.

Hence the first global buckling load factor to unfactored self-weight = 16.9. From plot, buckled mode shape shows primarily vertical displacement, as the normalization is 1000 mm and the vertical displacement reach up to 982.7 mm. The static displacement at the onset of buckling can be estimated by the following projection

[ ] {P }

∆{U} = λ K AE

−1

A n

This can be used to ascertain whether geometrically nonlinear effects or material nonlinearity for that matter, affects the estimation of the buckling load and the static displacement at the onset of buckling. The following is the static displacement from the unfactored self-weight load case.

188


The predicted max static displacement from the unfactored self-weight case at onset of buckling is 16.9 x 143mm = 2414mm Note that this is the max displacement, not the average. A geometrically nonlinear buckling analysis is required to predict a more accurate buckling load.

Linearized Buckling Due To ULS Load Case A (Max Downward Symmetrical Load 1.35Dead+1.5Snow With Applied Vertical Resultant 22530kN) The factor of safety on buckling to the ULS load case is of interest. The first realistic mode shape is presented. The load factor is 6.33.

As a check, from a linear projection of the self-weight case, since the distribution of load is similar, the load factor from this ULS case should be 9547 / 22530 * 16.9 = 7.15, not too dissimilar to the above prediction. The following is the static displacement from this ULS load case.

189


Hence, at the onset of buckling from the ULS case, from the above projection, the max static displacement is 6.33 x 382mm = 2418mm This is a 2.4m deflection in a span of 40m, i.e. span/depth of 16.5. The effect of this on the accuracy of the linear buckling load factor estimate needs to be quantified using a geometrically nonlinear buckling analysis solver.

Linearized Buckling Due To ULS Load Case B (Asymmetrical Load 1.35Dead+1.35Wind North+1.35Snow With Applied Vertical Resultant 21280kN) The North Wind load case refers to an asymmetric wind load case such that the windward direction experiences a downward pressure and the leeward direction experiences an upward pressure. The first realistic mode shape is presented. The load factor is 5.15.

Conclusion

190


The critical self-weight linearized buckling load factor is 16.9. Since the value is greater than 10.0, the effect of P-∆ in increasing the effects on the structure and reducing the load factor due to self-weight is negligible. The critical ULS linearized buckling load factor is 5.15. Since the value is less than 10.0, the effect of P-∆ in increasing the effects on the structure and reducing the load factor due to the ULS load case is not negligible. However the risk of catastrophic buckling instability is low.

Assumptions The following should be borne in mind when considering results. 1. Material linear and elastic until buckling. 2. Geometrically linear; Elastic stiffness KEA constant until onset of buckling and based on initial undeformed geometry; Valid if deflections small (for negligible change in KEA) until onset on buckling and no prestress (whether compressive which is unfavourable or tensile which is favourable) in structure. Check magnitude of ∆{U} to be small and ensure no prestress in system. 3. Geometrically linear; Geometric stiffness KGKEA based on KEA; Valid if deflections small (for negligible change in KEA and KGKEA) until onset on buckling. Check magnitude of ∆{U} to be small.

191


GL, ML (KGA From Exact or Approximate KTA) Buckling Analysis

3.2.4.2

The above subcase definitions will solve the following eigenvalue problem.

[[K

A E ]+

]

λ[ K GAKE ] {φ} = {0}

AKE

KG represents the geometric stiffness matrix which was calculated based on displacements obtained by solving the system with stiffness KEA. This may prove inadequate in many instances such as when there is prestress in the elements. The linearized buckling problem as described in the theory section is sought as

[[K

A T ]+

]

AKT λ[ K Gn ] {φ} = {0}

AKT

represents the geometric stiffness matrix which was calculated based on displacements obtained by solving KG the system with stiffness KTA. To obtain KTA, to be theoretically exact, a GNL SOL 106 (or implicit dynamic relaxation SOL 129 or explicit dynamic relaxation LS-DYNA) with prestress (as temperature loads say) and gravity must be undertaken. Alternatively, an approximation to KTA can be obtained by repetitive P-∆ static analyses with the prestress (as temperature loads say) and gravity applied. The procedure to obtain this approximate KTA will be presented. Note that the approximate KTA will be the summation of the elastic stiffness KE at the undeflected (by the prestress and gravity) state but KG at the deflected (by the prestress and gravity) state. Hence if KE changes considerably during the application of the prestress, a full SOL 106 (or implicit dynamic relaxation SOL 129 or explicit dynamic relaxation LS-DYNA), which converges to the KE and KG at the deflected (by the prestress and gravity) state should be employed. Hence for the modelling of a suspension bridge where there is a great change in geometry (known in the bridge industry as form-finding, so-called because it is necessary to find the form or shape of the catenary suspension cables), it may be prudent to employ SOL 106 (or implicit dynamic relaxation SOL 129 or explicit dynamic relaxation LS-DYNA), but for a high tension low sag cable on say a tower with prestressed cables, the repetitive P-∆ static analysis may be adequate. The repetitive P-∆ analysis basically involves a number of iterations of linear static analyses to obtain an approximate KTA. Note again that A refers to the initial undeflected (by the collapsing load) state, but deflected by the prestress and gravity. To perform the repetitive P-∆ analysis, a static analysis is performed based on KEA with temperature loads and gravity to generate forces in the structural elements, which in turn provides input for the computation of KGiAKTm where m is the iterations. Repetitive static analysis is performed with the prestress and gravity updating the stiffness matrix KEA + KGiAKTm-1 + KGiAKTm until convergence of displacements is obtained. The tangent stiffness at this stage is the approximate converged tangent stiffness matrix KTA = KEA + KGiAKT. The converged displacements represent the approximate P∆ (KGA From Approximate KTA) static response to the initial prestress loads. The converged geometric stiffness at this stage would be that based upon the approximate tangent stiffness matrix KTA, i.e. KGiAKT.

Phase 1 Perform static analysis (with prestress and gravity) based on [KEA] but include the segyroa.v2001 alter prior to the Case Control Section in order to compute the geometric stiffness matrix [KGA]1 (and output into a .pch file) based on the generated element loads from the [KEA] static analysis.

Phase 2 Perform static analysis (with prestress and gravity) based on [KEA] + [KGA]1 by including the k2gg = ktjj statement in the Case Control Section, the outputted .pch file which contains the ktjj matrix in the Bulk Data and the segyroa.v2001 alter prior to the Case Control Section to compute the [KGA]2 (and output into the .pch file overwriting previous data) based on the generated element loads from the [KEA] + [KGA]1 static analysis.

Phase 3 Repeatedly perform the Phase 2 static analysis (with prestress and gravity) based on [KEA] + [KGA]i for i = 2 to n where n represents the number of iterations required for the change in deflections between analyses to become

192


negligible. This would signify that the change in the [KGA] matrix become negligible and the correct [KGA] is attained. The deflections and the other responses at this stage represent the P-∆ (KGA From Approximate KTA) static response to the prestress and gravity. The stiffness of the structure is KTA.

Phase 4 Linearized buckling analysis is now performed with the stiffness of the structure at KTA and with a general buckling load. A SOL 105 is undertaken with the Case Control Section described as follows. It includes one more static analysis with the collapsing buckling load (a fraction of the critical load so that the load factor is more than 1) in order to generate the KGnAKT matrix. Then a buckling analysis is performed. $ CASE CONTROL SECTION SUBCASE 1 LABEL = P-∆ (KGA From Approximate KTA) Static Load Case With Buckling Load k2gg = ktjj LOAD = < ID of FORCEi, MOMENTi, PLOADi, GRAV, LOAD, SPCD Cards in Bulk Data > TEMP(LOAD) = < ID of TEMP, TEMPRB, TEMPP1 Cards in Bulk Data > DEFORM = < ID of DEFORM Cards in Bulk Data > SPC = < ID of SPC Cards in Bulk Data > SUBCASE 2 LABEL = Buckling Case k2gg = ktjj SPC = < ID of SPC Cards in Bulk Data > METHOD = < ID in EIGRL > $ BULK DATA Include ‘….pch file containing ktjj’

The responses at this stage represent the (KGA From Approximate KTA) linear buckling response. We have thus introduced so far 4 methods of getting the KTA matrix, namely full SOL 106, an implicit dynamic relaxation SOL 129, an explicit dynamic relaxation LS-DYNA or a repetitive P-∆ static analysis, all with the prestress and other loads. Once the KTA matrix is obtained, all that is required is to perform a linear static analysis with the buckling loads in order to generate a KGA (clearly from KTA) matrix. Now the linearized buckling problem can be solved as the linear eigenvalue problem [KTA + λKGA]{φ}={0}. Another approximate procedure can also be employed in order to generate the KTA matrix. $ CASE CONTROL SECTION SUBCASE 1 LABEL = Static Preload Load Case LOAD = < ID of FORCEi, MOMENTi, PLOADi, GRAV, LOAD, SPCD Cards in Bulk Data > TEMP(LOAD) = < ID of TEMP, TEMPRB, TEMPP1 Cards in Bulk Data > DEFORM = < ID of DEFORM Cards in Bulk Data > SUBCASE 2 LABEL = Static Load Case With Buckling Load LOAD = < ID of FORCEi, MOMENTi, PLOADi, GRAV, LOAD, SPCD Cards in Bulk Data > TEMP(LOAD) = < ID of TEMP, TEMPRB, TEMPP1 Cards in Bulk Data > DEFORM = < ID of DEFORM Cards in Bulk Data > SUBCASE 3 LABEL = Buckling Case STATSUB(PRELOAD) = 1 STATSUB(BUCKLING) = 2 METHOD = < ID in EIGRL >

193


The method is valid when only the prestress is judged to affect the geometric stiffness such as in the compressive preload of building columns due to gravitational loads and the prestressing of extremely taut cables that sag very little under gravity but not in systems such as suspension bridges. Where lateral loads are large enough to affect the geometry of the system with prestress, then a repetitive P-∆, SOL 106, implicit dynamic relaxation SOL 129 or explicit dynamic relaxation must be employed. But in single P-∆ analysis, because cables do not have much elastic bending stiffness, the initial static preload subcase should only include the prestress and not gravity as including gravity is the same as solving two linear static problems of stiffness KEA with preload and gravity as the applied loads respectively. Clearly, in the gravity case, it is nonsensical as the cables do in reality have differential stiffness (from the prestress) to resist the gravitational force. Prestress in one direction (i.e. along the axis of cable) will cause a differential stiffness in the orthogonal direction. Gravity acts in the orthogonal direction and hence cannot be accounted for in the calculation of the prestress in this single P-∆ analysis. To quantitatively decide if gravity need not be considered in contributing to the differential stiffness of the cables, a static P-∆ analysis should be carried out, the first subcase being a SOL 101 with only the prestress as applied loads and the second subcase a P-∆ SOL 101 (i.e. utilizing the induced prestress from the first subcase to form a geometric stiffness matrix) with both the gravity and prestress included as applied loads. If the difference in the cable element forces between subcases 1 and 2 is negligible, then gravity has little influence in affecting the geometric stiffness. If there is a major difference in the cable element force, then clearly, gravity will affect the geometric stiffness and as such, a repetitive P-∆ , SOL 106, implicit dynamic relaxation or explicit dynamic relaxation must be used to converge to the true KT. Likewise, in the single P-∆ analysis of multi-storey buildings, gravity (and only gravity) acts in axis of columns to generate prestress, and the differential stiffness is computed for the orthogonal direction reducing resistance to lateral wind forces, applied in the second subcase with gravity too. The STATSUB(PRELOAD) computes the differential stiffness due to the prestress and also the follower force. The follower force is calculated and incorporated by the use of PARAM, FOLLOWK, YES. We know how the prestress affects the differential stiffness, namely a tensile prestress causing an increase in stiffness. The effect of the follower force on the stiffness is different. For example, for a cylinder under external pressure critical buckling load may be overestimated (even though the mode shapes are similar) in a SOL 105 and the natural frequencies in vibration may be underestimated (even though the mode shapes are similar) in a SOL 103 in the absence of follower stiffness. To the contrary, these observations are reversed in case of centrifugal loads. Centrifugal forces as a constant (static) load are applied by a Bulk Data RFORCE to any elements that have masses. The follower stiffness due to centrifugal load has the effect of lowering stiffness (although the centrifugal load tensioning effect increases stiffness), consequently lowering natural frequencies (even though the mode shapes are similar) in a SOL 103 and lowering the buckling loads (even though the mode shapes are similar) in a SOL 105. This effect increases as the RPM increases, and it becomes significant when the RPM is over 1000. Another important observation is that the preload cannot buckle the structure. The basic eigenvalue problem was expressed as where λ is an eigenvalue which is a multiplier to the applied load to attain a critical buckling load. If there exists constant preloads other than the buckling load in question, the above equation should include additional differential stiffness, i.e.

in which differential stiffness is distinguished for constant preload and variable buckling load. Notice that no eigenvalue solutions are meaningful if the preload makes the structure buckle, i.e. should be positive definite.

194


3.2.5

Hand Methods Verification Member or Local (KGA From KEA) Buckling

3.2.5.1 3.2.5.1.1

ML, GL Euler Buckling of Column Elements (Primary Stress is Only Axial)

The Euler equation for the critical elastic buckling load for an elastic, isotropic and straight column is PE =

π 2 EI LE

The Euler load estimate is perfectly analogous to the SOL 105 buckling load estimate.

2

where LE is the effective length (distance between the points of contraflexure) depending on the boundary conditions. Boundary Conditions Effective Length, LE Non-Sway Sway Pinned-Pinned 1.0L (Truss) Pinned-Rigid 0.699L 2.0L Rigid-Rigid 0.5L 1.0L The Euler equation is of course only valid for columns that are sufficiently long enough to experience linear elastic instability before yielding. Hence it is better to work in terms of axial stresses as the yield stress is clearly defined. The critical Euler stress is π2E I σE = where r = 2 A (L E / r ) It cannot be emphasized enough that, the and is only valid if theoretical buckling load factor is independent of the initial lateral imperfections, the lateral LE π2E load and material strength. > r σy This is all illustrated in the following diagram. σ cr σ cr = σ y σy π2E σ cr = (L E / r )2

The curves are fully described by the Rankine σy buckling formula σ RANKINE = σy  L 2 1+ 2  e  π E r  Slendernes s

LE = r

π2E σy

LE r

The buckling stress capacity depends on the stiffness of the element and the boundary conditions, both of which is accounted for in the slenderness parameter LE/r. For low slenderness, the beam fails by yielding, and for high slenderness, it fails by buckling. This slenderness parameter should be checked for both the major axis and the minor axis as the boundary conditions may differ. The capacity corresponding to the greater slenderness is clearly critical. The critical load capacity is PE = σ E A

The Euler buckling load presented hitherto is actually the flexural Euler buckling load π 2 EA PE = σ E A = (L E / r )2

195


There is also the much smaller possibility of shear buckling. When buckling occurs, shear forces act on the section. These give rise to additional shear deformations that reduce the force that the member can take in compression before it becomes unstable and buckles.

The critical load for combined flexural and shear buckling is given by 1/Ncrit = 1/Ncrit.flexural +1/Ncrit.shear Hence, the critical force is reduced approximately by the factor 1/[1+Ncrit/GAs), where Ncrit is the critical force in the absence of shear deformation. On top of Euler flexural and shear buckling, columns are also subject to torsional buckling and flexuraltorsional buckling. These occur when the ratio of torsional to flexural stiffness is very much reduced.

196


3.2.5.1.2

ML, GL Lateral-Torsional Buckling of Beam Elements (Primary Stress is Only Bending)

From classical mechanics, it can be shown that the lateral torsional buckling capacity for an elastic, isotropic beam with a uniform bending moment diagram is M LTB =

π LE

EI MINOR GJ 1 +

π 2 EI w

The LTB load estimate is perfectly analogous to the SOL 105 buckling load estimate.

L2E GJ

I w = warping stiffness = I MINOR

h2 for an I - section 4

The lateral-torsional buckling of a beam is governed by both the minor axis elastic second moment of area, IMINOR and also the torsional constant, J. Contrast with the Euler buckling which depended upon only the minor axis elastic second moment of area, IMINOR. The π is replaced with another value depending on the bending moment diagram; 4.24 for a triangular BMD due to a central point load; 3.53 for a uniform uniformly distributed load BMD. However, beams are subject to plastic failure (attainment of plastic moment capacity) at low slenderness and to lateral torsional buckling at higher slenderness. The plastic moment capacity is M plastic = S plastic σ y

It cannot be emphasized enough that, the theoretical buckling load factor is independent of the initial lateral imperfections, the lateral load and material strength.

This is all illustrated in the following diagram. σ cr σy

σ cr =

M plastic S plastic

= σy σ cr =

M LTB S plastic

Slendernes s

LE r

The buckling stress capacity depends on the stiffness of the element and the boundary conditions, both of which is accounted for in the slenderness parameter (LE/r). For low slenderness, the beam fails by yielding, and for high slenderness, it fails by lateral torsional buckling. Lateral torsional buckling cannot occur in beams loaded in their weaker principal plane; under the action of increasing load they will collapse simply by plastic action and excessive in-plane deformation. Hence, the check need only be made for bending about the major axis.

197


3.2.5.1.3

ML, GL Euler Buckling of Plate Elements

Theoretical solution for the Euler buckling of a plate (panel) of thickness t, width of b and the two loaded edges simply supported is a kπ 2 E b σE = 2 12 1 − ν 2 (b / t ) where k is dependent upon the boundary conditions of the two non-loaded edges and also on the ratio of a/b, where a is the length of the panel. The table below presents the minimum values of k for different boundary conditions of the unloaded edge, with the loaded edge simply supported.

(

)

Unloaded Edge Condition Both fixed One fixed, one simply supported Both simply supported One fixed, one free One simply supported, one free

k 6.970 5.420 4.000 1.280 0.425

Unlike columns, plates do not collapse when the critical buckling load is achieved. Constraints due to the twodimensional nature of the plates allow plates to resist increasing loads beyond buckling. Hence the nonlinear postbuckling analysis is more important for plates. In BS 5950-Part 1:2000, cross-sections are classified to determine whether local buckling influences their capacity, without calculating their local buckling resistance. The classification of each element of a cross-section subject to compression (due to a bending moment or an axial force) should be based on its width-to-thickness ratio. The section classes are as follows.

Class 1 Plastic: Sections with plastic hinge rotation capacity. The full plastic modulus S may be used in design. Class 2 Compact: Sections with plastic moment capacity. The full plastic modulus S may be used in design. Class 3 Semi-Compact: Sections in which the stress at the extreme compression fibre can reach the design strength, but the plastic moment capacity cannot be developed. Elastic design methods must be adopted, i.e. the full elastic modulus Z must be used in design. Class 4 Slender: Sections in which it is necessary to make explicit allowance for the effects of local buckling. BS 5950-Part 1:2000 gives approximate methods using an effective area for Z calculation in cl. 3.6.

198


Section Classification BS 5950-Part 1:2000 Design strength of steel, py = f(steel Grade, thickness) (N/mm2) For Class 1, 2, 3, the outstand element of rolled compression flange b/T (half of the width of flange divided by the flange thickness) must be < 9ε, 10ε, 15ε For Class 1, 2, 3, the internal element of compression flange b/T (width of attached plate on flange divided by thickness of attached plate) must be < 28ε, 32ε, 40ε For Class 1, 2, 3, the outstand element of welded compression flange b/T (width of the outstand portion of attached plate on flange divided by the thickness of the attached plate) must be < 8ε, 9ε, 13ε For Class 1, 2, 3, an angle or the outstand of an angle connected onto another component b/t and d/t must be < 9ε, 10ε, 15ε

cl. 3.5 Table 9 Table 11 or Table 12 Table 11 or Table 12 Table 11 or Table 12 Table 11 or Table 12

For Class 1, 2, 3, the stem of a T- section D/t must be < 8ε, 9ε, 18ε

Table 11 or Table 12

For Class 1, 2, 3, the web of I-, H- or Box section d/t must be < 80ε, 100ε, 120ε


For Class 1, 2, 3, the web of a channel section d/t must be < 40ε, 40ε, 40ε


For Class 1, 2, 3, CHS must have D/t < 40ε , 50ε , 140ε


For Class 1, 2, 3, RHS must have b/t < 28ε, 32ε, 40ε and d/t < 64ε, 80ε, 120ε


2

2

2

Note that ε = (275/py) . 0.5

Note the much tighter criteria (about 9ε, 10ε, 15ε) for local sections which are not constrained such as the outstand of a flange, an angle or the stem of T- section. Note the fairly relaxed criteria (about 40ε, 40ε, 40ε) for partially constrained sections such as the web of a channel. And note the very relaxed criteria (about 80ε, 100ε, 120ε) for constrained sections such as the web of a I-, H- or Box section.

199


200


201


3.2.5.1.4

Web Shear Buckling

Web Shear Buckling BS 5950-Part 1:2000 Ensure d/t < 62ε for welded sections or 70ε for rolled sections to avoid web shear buckling

cl. 4.4.5

Additional considerations to moment capacity must be made according to cl. 4.4.4.2 if web is subject to shear buckling.

202


3.2.5.2 3.2.5.2.1

Overall System (KGA From KEA) Buckling Linear Elastic Buckling Based on Energy Principles

203


204


205


206


207


208


209


210


211


212


3.2.5.2.2

ML, GL Approximate Bifurcation (Linear Buckling) Analysis of Multi-Story Frames

The approximate bifurcation analysis of multi-story frames estimates an approximate elastic critical load, λECR.

BS 5950-Part 1:2000 (cl. 2.4.2.6) gives a method for calculating λcr for simple (symmetric in plan) multi-storey buildings (excluding single-storey frames with moment-resisting joints and other multi-storey frames in which sloping members have moment-resisting connections) based on the deflection due to the Notional Horizontal Forces of 0.5% of the factored vertical (1.4 dead + 1.6 live) load or 1.0% of the factored vertical (1.4 dead) load, whichever the greater applied at the same level. λ cr =

1 h 200 δ

where h/δ is the value of the storey height divided by the deflection over that storey (deflection at top of storey relative to deflection at bottom of storey) for any storey in the building. The smallest value considering every storey should be used. This equation is based on a shear mode buckling and gives very good agreement with more detailed analysis. Lower buildings tend to be governed by shear buckling whilst taller buildings are governed by the flexural buckling mode. If the mode is flexural, the above simple equation is likely to underestimate (conservative) λcr. The stability systems for steel buildings are often braced cores. It can be shown that if the stress in the diagonals is greater than 57MPa, however stiff the columns and beams, λcr will be less than 10.

213


3.3 3.3.1

GL, MNL Plastic Collapse Analysis by the Implicit Linear Simplex Programming Mathematical Formulation of Analysis

Great structural engineering failures since time immemorial can be attributed to a lack of redundancy. A plastic collapse analysis is a brilliant method of finding out the amount of redundancy that a structure had to a load. λ

ML, GL Static Analysis ML, GL Buckling Analysis λECR ML, GL P-∆ Static Analysis ML, GNL Static and Buckling Analysis (Tracing Equilibrium Path or Implicit or Explicit Time Integration with Dynamic Relaxation) MNL, GL Plastic Collapse Analysis λP MNL, GNL Static and Buckling Analysis (Tracing Equilibrium Path or Implicit or Explicit Time Integration with Dynamic Relaxation) λF U


Plastic collapse analysis is performed if material non-linearity (yielding and subsequent formation of plastic hinges) is thought to be more significant than elastic buckling instability in causing the failure of the structure. The structure has not buckled (experienced elastic instability) but has α + 1 fully plastic hinges, i.e. a mechanism. In order to use plastic collapse analysis methods, the beams and columns must be ductile, i.e. must be able to deform sufficiently to form plastic hinges. Ductility in beams improved by having less than 4% steel reinforcement, having shear links to confine concrete in three dimensions, having a little compression steel, too much of which will reduce ductility. Ductility in columns improved by having shear links to confine concrete in three dimensions to avoid the propagation of micro-cracks. The Uniqueness Theorem states that the smallest critical plastic collapse load factor is attained if the 3 following condition are achieved: I. Equilibrium condition: The bending moment distribution must be in equilibrium with the external applied loads II. Yield condition: The bending moment must nowhere exceed the plastic moment capacity of the section III. Mechanism condition: There must be sufficient plastic hinges to form a mechanism. The Upper Bound Mechanism Method of Plastic Limit Analysis to find λP uses the equilibrium conditions and postulates many collapse mechanisms, finding the critical combination by minimizing λP. If the postulated collapse mechanisms subsumes the critical one, then the collapse bending moment diagram will show that no part of the structure does the moment exceed the plastic moment capacity, i.e. the yield condition would have been met.

min λ λOPT The proposed plastic collapse analysis is a geometrically linear method. Often, P-∆ effects (reduction in lateral bending stiffness of axially loaded columns) need to be accounted for. We could approximately incorporate geometric non-linearity to find an approximate λF by employing Wood’s adaptation of the Merchant-Rankine empirical formula based on an estimate of the critical elastic load factor, λE. Note also that should the axial forces be large in certain elements, the value of the plastic moment capacity MP would decrease in accordance with the MN diagram.

214


The analysis is performed as follows (i)

Select critical sections C or C* (i.e. whether simple frame or multi-bay multi-storey frame), identify degree of static indeterminacy α or α* (i.e. whether simple frame or multi-bay multi-storey frame), and establish the sign convention for positive bending moments and rotations. Select critical sections C i.e. potential plastic hinge locations -

-

fixed supports joints between members - between two members without applied moment, only one possible critical section at the joint, i.e. at the weaker member - between two members with applied moment, two possible critical sections - at a 3 or more member joint, all the member ends must be included as possible critical sections under concentrated loads under uniform loads at changes of member detailing, i.e. discontinuity in MP and plastic hinge occurs in weaker section

Degree of static indeterminacy for plane frames = 3 (number of windows) – releases r Degree of static indeterminacy for space frames = 6 (number of windows) – releases r Degree of static indeterminacy for grillages = 3 (number of windows – 1) – releases r

Hyperstatic

Isostatic

Statically indeterminate, α > 0

Statically determinate, α = 0

Many stress paths from any point to root

Only one stress paths from any point to root

One or more mesh or closed loop

No mesh or closed loop

Bending moments and rotations are defined as positive if they cause tension or extension at the side with the dotted lines. For multi-storey multi-bay buildings, the dotted line is drawn under beams and on the right of columns by convention. (ii)

Formulate the equilibrium law equations Draw bending diagrams (employing sign convention) on released structure for: (a) Releases p1, p2, p3 … (b) External load parameter λ

p  m C = [B b 0 ]  α  λ 

 m1   B  .  .  =  .  .     mC   .

p  b0   1   B . .     .  . = . . . .   .  p  . . B b0   α   .  λ  . . . .

. .

215

.   p1  b0    .  .  .  + λ  . . . .  .      . . B.  pα  b0  . . . .


(iii) Formulate the mesh kinematic linear program for the plastic limit analysis

 b T − b T0  & 1 T θ =  minimise λ = M P θ&* 2C subject to  T0 T * 0 B − B  positivity condition θ&* ≥ 0 (iv)

Solve the linear program using the Simplex method

(v)

Determine the uniqueness of the collapse mechanism

(vi)

Determine the uniqueness of the bending moment diagram at collapse

(vii) Establish the bending moment distribution at collapse from the equilibrium equations (viii) Establish the actual elastic and plastic deformations (i.e. rotations and displacements) [Ba]T{θPa} = −[B]T[f]{m} [Ba] = mesh matrix associated with active plastic hinges {θPa} = active plastic hinges vector [B] = complete mesh matrix [f] = flexibility matrix {m} = bending moment at collapse vector {d} = [B0]T {{θE}+{θPa}} = [B0]T {[f]{m}+{θPa}} {d} = displacement vector [B0] = matrix equilibrating a unit load without compatibility considerations at each and every station where the deflection is sought (ix)

Employ the approximate bifurcation analysis for simple frames or other methods to find an approximate λECR

Steven ' s Estimate

λ ECR = 0.9

∑S h φ ∑V h φ i i

Horne' s Estimate (x)

λ ECR = 0.9

i i 2 i i

S/ V Max φi

Employ Wood’s adaptation of the Merchant-Rankine empirical formula to find an approximate λF. This effectively accounts for the P-∆ (KGA From KEA) effect from the linear elastic buckling load, which is based on the initial undeflected geometry.

λF = λP

1 λ 0.9 + P λ ECR

λF = 1 for λP

for

4≤

λ ECR ≤ 10 λP

λ ECR ≥ 10 i.e. assume no geometricnonlinearity effect beyond ratio of 10 λP

Note that in conceptually well designed structures, λECR >> λP such that λF ~ λP (Merchant-Rankine). Also, λE << λP so that the structure deforms considerably in plasticity before failure.

216


3.3.2

Mathematical Proof

Equilibrium law equations

 p m = [B B 0 ]   λ 

 m1   B  .  .  =  .  .     mC   .

. . . .

. .

B0 .

. .

. . . . . B

. .

. .

 p1   .   .    . .    p .  α   λ  B0   1   .  λ   total 

Incorporating the single parameter loading λ, the equilibrium law equations become

 p m = [B b 0 ]   = B p + λ b 0 λ   m1   B  .  .  =  .  .     mC   .

p  b0   1   B . .     .  . = . . . .   .  p  . . B b0   α   .  λ  . . . .

. .

.   p1  b0    .  .  .  + λ  . . . .  .      . . B.  pα  b0  . . . .

Kinematic law equations by the static-kinematic duality law

 v&  B T  & δ& =  T ϑ   B 0 

 v&1   B T  .      .  .   .     v&α  =  .  δ&1   B0T     .   . δ&   .  total  

. . . . . . . . . . . . . .

217

.   .  & θ  .  1   . BT    .  .  &  θ  .  C  B0T 


Incorporating the single parameter loading λ, the kinematic law equations become

 v&   B T  & W&  =  T ϑ  λ =1   b 0 

 v&1   B T  .      .  . = .     v&α   . W&λ =1   b0T Mechanism compatibility law

.  &  θ  .  1  . .    .  BT  &  θ  b0T   C 

. . . . . .

. . . .

[0] = [B T ]ϑ& 0  B T .   = . .  .    0  .

  θ& 1    .   .    . . B T  θ&C  . . . . . .

. . .

Rate of Work T W&= λ δ& T T W&= λ B 0 θ&from the kinematic law

[ ] W&= [λ B ]θ& T

T 0

T W&= [B 0 λ ] θ& T W&= [b λ ] θ& 0

T W&= λ b 0 ϑ& T at unit load factor, W&λ =1 = b 0 ϑ&

Rate of Energy Dissipation

&= M T θ& , D P *

[

&= M +1 . . M +C D P P

θ&* ≥ 0

M P−1 . . . M P−C

218

θ&*+1     .   .   &+C  θ *  ,  θ&−1   *   .   .    θ&*−C 

]

θ&* ≥ 0


The rate of energy dissipation terms are always positive. Also, only one of the angle terms (of the +ve and –ve superscripted angle terms) for each particular critical section should be included in the rate of energy computation. Flow Rule

θ&= Nθ&* ,

θ&* ≥ 0

θ&*+1     .  θ&  1 −1  .  1      &+C  −1  . = 1  θ * ,  .     θ&*−1  1 −1   &   − 1  .  1 θ C    .    θ&*−C 

θ&* ≥ 0

Mesh Kinematic Linear Program for Plastic Limit Analysis

For collapse, &= D & W

λ b T0 ϑ&= M P T θ&* ,

θ&* ≥ 0

but θ&= Nθ&* , θ&* ≥ 0 λ b T0 Nθ&* = M P T θ&* , θ&* ≥ 0 T b Nθ& = 1 (normalisation condition) 0

*

T ∴ λ = M P θ&* ,

θ&* ≥ 0

Hence, the mesh kinematic linear program for plastic limit analysis is minimise λ = M T θ& P

b  B positivity condition

subject to

T 0 T

*

− b  & 1  (1 equation for normalisation condition, 2C terms) θ * =   −B  0 (α equations for mechanism compability, 2C terms) θ& ≥ 0 T 0 T

*

219


Rewriting, the mesh kinematic linear program for plastic limit analysis is

minimise

subject to

[

λ = M +P1 . . M +PC

 bT  0T B  .   .  T B α

M −P1 . . . M −PC

. .

b T0

C

− b T0

. .

. . . .

BC .

T

− BT .

. . . .

. T − Bα

. . . .

. . . T . . B α,C

+ − positivity condition θ&* ≥ 0, θ&* ≥ 0

220

 θ&*+1     .   .   +C  θ&*   θ&−1   *   .     .  θ&*−C 

]

 θ&*+1    .  T C  1 − b0  .    T − B C   &+ C  0 θ *  .   &−1  = 0 θ*    0 .  T  .    − B α ,C    0 .   θ&*−C 

(1 equation for the normalisation condition with 2C terms, and α equations for mechanism compability with 2C terms)


3.3.3

Displacements and Rotations at Collapse

221


3.3.4 3.3.4.1

Plastic Limit Analysis of Simple Framed Structures Portal Frame

Given simple frame with beam 2MP and columns MP subject to vertical 4λ and horizontal 1λ loading as shown. The plastic collapse load factor is required. Select critical sections C (shown by the blackened circles), identify the degree of static indeterminacy α, and establish the sign convention for positive bending moments and rotations. For bending moments, tension is positive and for rotations, extension is positive. 4λ 3

2

λ

4 L

1

α=2 C=4

2L Draw bending diagrams (employing sign convention) on released structure for releases p1, p2 and external loads defined by single parameter loading λ. We only need a load-equilibrating BMD (that not necessarily satisfies compatibility) for the external load whilst the BMD for the releases should satisfy compatibility. The flexural analysis for the releases p1 and p2 does not include the external loads, whilst that of λ naturally does. One solution would be to release two rotational freedoms at 1 and 3 such that a three-pinned-arch is formed. The releases of an internal action would necessitate the use of a bi-external action to define the p-action diagram. For instance, the releases of an internal bending moment would require the use of a bi-external moment to define the p-BMD. Formulate the equilibrium law equations. Leave the b0 matrix vector numerical, hence placing the variables λ, L etc in the RHS release-loading vector. 4λ P 2 -0.5 0 -1.5 -2.5 0 λ 1 1 0.5 1 1

0

0

P1 P1=1 diagram

P2=1 diagram

λ=1/L diagram

1 0 0   m1   1 3  m  1 −   p1   2 p   2 = 2  m3   0 1 0   2    − 1 1 − 5  λL   m4   2 2

p  m C = [B b 0 ]  α  λ 

Formulate the mesh kinematic linear program for the plastic limit analysis of the frame. Leave MPT numerical. All MPT values are positive and are repeated in the latter half of the row vector.  b T − b T0  & 1 T minimise λ = M P θ&* 2C subject to  0T θ =  T * 0  B − B  positivity condition θ& ≥ 0 *

222


 θ&*+1   &+ 2   θ*  θ&+3 .  &*+ 4  θ minimise z = [1 1 2 1 1 1 2 1] *−1  subject to θ&  −* 2   θ&*   &−3  θ* .  θ&*− 4 

3 5  0 − 2 0 − 2  1 1 1 0 − 2 2  0 1 1 1 

3 2 1 −1 − 2 0 −1 0

 θ&*+1   &+ 2  θ 5   +*3   0 θ& . 2   *+ 4  1 1   θ&*     = 0 0 2   θ&*−1    − 1 − 1  &−2  0   θ*  &−3 θ* .  θ&*−4 

M positivity condition θ&* ≥ 0 and note that λ MIN = z MIN P since M TP and b 0 were left numerical. L Alternatively, numerical values could have been used for MP and L, in which case λMIN = zMIN. Set up and solve the linear programme (LP) in a Simplex Solver. PLASTIC MOMENT OF RESISTANCE, MP 1 1 2 1 KINEMATIC MATRIX 0 -1.5 1 0.5 0 1 VARIABLES, θ 0 0

0 0 1

0.4

-2.5 -0.5 1

0

OBJECTIVE FUNCTION TERMS (= MP x θ) 0 0 0.8 0 CONSTRAINT 0 0 0

1

0 -1 0

1

2

1

1.5 0 -0.5 0 -1 -1 Cells to change

2.5 0.5 -1 Target cell to minimize

0.2

0

0

0.4

0.2

0

0

0.4

0 0 0

1 0.2 -0.4

SUM

FUNCTION TERMS (= KINEMATIC MATRIX x θ) 0 0 0 0 0 0 0 0 -0.2 0 0 0.4 0 0 0

SUM

Constraints

Also include positivity condition

The changed cells in red represent the solution. The Sensitivity Report will also be produced by the solver. Microsoft Excel 9.0 Sensitivity Report Worksheet: [simplex - plastic collapse analysis.xls]Sheet1 Report Created: 26/05/2003 17:02:57

Adjustable Cells Cell Name $A$10 VARIABLES, θ $B$10 $C$10 $D$10

Final Reduced Objective Allowable Allowable Value Cost Coefficient Increase Decrease 0 2 1 1E+30 2 0 1.6 1 1E+30 1.6 0.4 0 2 4 1 0 2 1 1E+30 2

223

1.4

1 0 0


$E$10 $F$10 $G$10 $H$10

0.2 0 0 0.4

0 0.4 4 0

1 0.5 1 1E+30 2 1E+30 10.666666667

2 0.4 4 2

Constraints Cell Name $J$16 SUM $J$18 SUM $J$17 SUM Constraints Cell Name $J$16 SUM $J$18 SUM $J$17 SUM

Final Shadow Constraint Allowable Allowable Value Price R.H. Side Increase Decrease 1 1.4 1 1E+30 1 0 2 0 1E+30 0.4 0 -1 0 0.2 1E+30

Cell Value

Formula 1$J$16=1 0$J$18=0 0$J$17=0

Status Slack Binding 0 Not Binding 0 Binding 0

We shall interpret the results and the Sensitivity Report. (a) The collapse load factor λMIN and plastic hinge angular velocities θ at collapse λMIN = zMIN MP / L = 1.4 MP / L (take MP = 1 and λ = 1 if they have been included numerically) θ∗+1 0

θ∗+2 0

θ∗+3 0.4

θ∗+4 0

θ∗−1 0.2

θ∗−2 0

θ∗−3 0

θ∗−4 0.4

(b) Current basic variables, potential basic variables (but as of the final tableau still non-basic) and non-basic variables recognition Current basic variables (participating or non-participating plastic hinges) could be zero (non-participating) as well as have a non-zero (participating) value. Hence, current basic variables (i.e. variables in the basis in the final tableau) are recognized by the fact that they: (i) have finite (zero inclusive) allowable increase in cost coefficient MPj Note that current basic variables can have zero or non-zero final values. Current basic variables will definitely have zero reduced cost values. Non-basic variables include all variables that are not basic variables. Non-basic variables are recognized by the fact that they: (i) have infinite allowable increase in cost coefficient MPj, Note that non-basic variables will definitely have zero final values. Non-basic variables can have reduced cost values of zero or non-zero. Potential basic variables (but as of the final tableau still non-basic) are recognized by the fact that they: (i) are non-basic variables, hence contain all recognition conditions of non-basic variables as above, AND (ii) have zero reduced cost

Basic variables

Non-basic variables

Potential basic variables

224


(c) Reduced costs The reduced costs are the objective function coefficients in the optimal tableau. For each variable xj (or θj), the reduced cost gives the increase in the target cell (z) for a unit change in the variable xj (or θj). Hence, if we take a non-basic (which is not a potential basic variable) angular velocity θ∗ and increase it by a unit, this would cause λ to increase by the reduced cost and hence λ would no longer be optimal. Reduced cost C j =

∂z ∂θ&*j

The reduced cost values associated with the basic variables (plastic hinge velocities) must be zero. However, if any reduced cost is zero for a non-basic variable, there can be an alternate collapse mechanism having the same load factor because this non-basic variable could be brought into the basis to form another collapse mechanism without increasing the plastic collapse load factor. (d) Allowable increase and allowable decrease The allowable increase is the amount by which the objective function coefficient cj (MPj) in the original tableau may increase before the value of xj (or θj) in the optimal solution is changed. For a non-basic variable, cj (MPj) can vary between min cj and +∝ before the xj (or θj) value is changed. Basic variables on the other hand have finite (zero inclusive) allowable increase values for its corresponding coefficients. (e) Shadow prices (a.k.a. Lagrange multipliers or dual variables) There is a shadow price associated with each constraint. The shadow price measures the change in the objective function z due to a unit change in the RHS of the constraints bi. But then, in this context of plastic limit analysis, the RHS of the constraints are either 0 or 1. ∂z Shadow price ∏ i = ∂b i The shadow price corresponding to the normalization constraint is the collapse load factor as obtained earlier. More importantly, the shadow prices associated with the mechanism compatibility constraints are the indeterminate forces from which the bending moment distribution at collapse can be ascertained. There is an indeterminate p force value for every mechanism compatibility constraint. It is crucial that the p value is associated with its corresponding constraint. Hence the manner in which the constraints are inserted into the Excel Solver tool determines the manner in which the p values are outputted. Note the cell name column in the constraints table for clarification. Here λ = 1.4MP / L, p1 = −1MP and p2 = 2MP. (f) Uniqueness of collapse mechanism The existence of a potential basic variable (but as of the final tableau still non-basic) confirms the nonuniqueness of the collapse mechanism. Other potential collapse mechanisms involve the activation of these potential basic variables (but non-basic as of the final tableau). The true collapse mechanism will involve some form of addition of all these potential plastic collapse mechanisms, i.e. MTRUE = α1M1 + α2M2 + α3M3 +… The existence of non-uniqueness in the collapse mechanism usually occurs when there are two concentrated loads of equal magnitudes acting on a beam and so causing two potential partial collapse mechanisms with the true collapse mechanism being the addition of the two, i.e. a complete collapse mechanism. (g) Uniqueness of bending moment diagram (BMD) at collapse The uniqueness of the BMD can be tested on a potential collapse mechanism or even the true collapse mechanism. The uniqueness of the collapse mechanism and the uniqueness of the BMD are independent properties. A collapse mechanism has a unique BMD if and only if it is a complete collapse mechanism, i.e. it has α+1 active participating (non-zero) angular velocities of plastic hinges. Note that some basic variables are zero and they cannot be included as one of the α+1 active participating hinges. The uniqueness of the BMD comes from the fact that having α+1 known MP locations will allow α+1 equations in the equilibrium law define uniquely the values of λ, p1, p2 … pα. However, if there are not α+1 active plastic hinges (and hence no unique BMD as the structure is statically indeterminate at collapse), then any BMD that satisfies equilibrium

225


will be on the safe side and can be accepted for design. Hence we could just use the shadow price values (of λ, p1, p2 … pα) off Excel in the equilibrium equations for a BMD. (h) Bending moment distribution at collapse

p  m C = [B b 0 ]  α  λ  m1   11 m    2 =  2 m 3   0    1 m 4  − 2

0   1 3   p1   1 1 −  2 p  =  2 1 0  2  0 5  λ L   1 1 −    − 2  2 0

0    − 1.0M P  3 1 −   − 1M P  − 0.6M  P 2  2M  =  P   2.0M P  1 0  5  MP    1 −  1.4 L L  − 1.0M P  2 0

Check that the bending moment everywhere is less than the particular plastic moment of resistance of the member. If so, we have correctly chosen the critical sections C that will produce the smallest value of λ. And hence the Yield Condition is met and λ is the unique collapse load factor according to the Uniqueness Theorem. To reiterate the above results for ease of understanding, we make the following observations in this order: I. II.

The critical plastic load factor is λP = 1.4 MP / L shown in the target cell to minimize and again in the Shadow Price of the Sensitivity Report. Identify the basic variables, i.e. the locations that a plastic hinge forms to form the collapse mechanism. This is identified in the Sensitivity Report on variables with a Finite (zero included) Allowable Increase. Here, they are θ3, θ1 and θ4, the latter two of which are negative. This means that they rotate such as to cause compression on the positive sign convention side. Usually (but not necessarily) the basic variables will be non-zero.

4λ 2

λ

3

4

1

III.

The value of the Allowable Increase is the amount by which the objective function coefficient i.e. the MP value corresponding to the basic variable can increase before the solution (i.e. values of the angular velocity θj) changes. This is useful to force another (maybe less catastrophic) collapse mechanism. To do this the structural engineer would have to increase the MP value at section 3 by 4MP, or at section 1 by 0.5MP or at section 4 by 0.67MP. Clearly, if say the engineer does not want the column to collapse (that being catastrophic), he would have to increase the MP of the column at section 1 to a little over 1.5MP. If that were done, in this case, sections 2, 3, and 4 would then form the mechanism, i.e. a less catastrophic beam mechanism. Next, we look for the existence of an alternate collapse mechanism. For each variable θj, the reduced cost gives the increase in the target cell (z) for a unit change in the variable θj. Thus the reduced cost of all the basic variables, i.e. the plastic hinges must be zero for the optimal conditions (i.e. minimum λ). Thus, if any reduced cost is zero for a non-basic variable (infinite Allowable Increase), there can be an alternate collapse mechanism having the same load factor because this non-basic variable could be brought into the basis to form another collapse mechanism without increasing the plastic collapse load factor. Here there is not any alternate collapse mechanism since all the variables with infinite Allowable Increase have non-zero Reduced Costs.

226


IV.

Finally we draw the BMD at collapse.

p  m C = [B b 0 ]  α  λ

 m1   11 m    2 =  2 m 3   0    1 m 4  − 2

0   1 3   p1   1 1 −  2 p  =  2 1 0  2  0 5  λ L   1 1 −    − 2  2 0

0    − 1.0M P  3 1 −   − 1M P  − 0.6M  P 2  2M  =  P   2.0M P  1 0  5  MP    1 −  1.4 L L  − 1.0M P  2 0

Check that the bending moment everywhere is less than the particular plastic moment of resistance of the member. If so, we have correctly chosen the critical sections C that will produce the smallest value of λ. And hence the Yield Condition is met and λ is the unique collapse load factor according to the Uniqueness Theorem. If the yield condition were not met, we would have reduced the estimate of critical plastic collapse factor as follows. M Exceeding λ Pr educed = λ P MP And we would say that the true critical collapse load factor lies between λ Pr educed < λ Ptrue < λ P

227


3.3.4.2

Parabolic Arch

Given MP = 590kNm

228


3.3.4.3

Displacements and Rotations at Collapse

229


230


3.3.5

Plastic Limit Analysis of Rectangular Multi-Storey Multi-Bay Frames with Improved Data Generation

(a) Select critical sections inclusive of articulation C*, identify the degree of static indeterminacy with articulation ignored α∗, and establish the sign convention for positive bending moments and rotations Critical sections inclusive of articulation C* are identified. α for plane frames with articulation = 3 (number of windows or cells) – releases r α∗ for plane frames with articulation ignored = 3 (number of windows or cells) Bending moments and rotations are defined as positive if they cause tension or extension at the side with the dotted lines. For multi-storey multi-bay buildings, the dotted line is drawn under beams and on the right of columns by convention. (b) Formulate the equilibrium law equations

p  m C * = [B b 0 ]  α *   λ  (i) 3 self equilibrating BMDs (due to shear, bending and axial actions) for each cell (sign convention applies) Note that C* is the number of critical sections inclusive of those originally articulated and α∗ is the degree of static indeterminacy with all articulation ignored. The articulation positions will thus also be regarded and denoted as critical sections. Hence, each cell will contribute 3 indeterminate forces and hence 3 columns in the B matrix. Fill in the B matrix column-by-column with the bending moment values of the 3 normalized cell self-equilibrating BMDs at the critical section positions of C*. (ii) 1 load equilibrating BMD for the load factor λ (sign convention applies) Vertical loads are transferred through simply supported beams, and hence MMAX = PL/4 if central load. Horizontal loads are transferred through cantilever action and multiple loads on the same column have their independent BMDs superimposed upon each other. (c) Formulate the mesh kinematic linear program for the plastic limit analysis of the frame and solve the LP Set the MP value of the real articulation (hinges) to zero in the MPT matrix.

 b T − b T0  & 1  T θ =  minimise λ = M P θ&* 2 C* subject to  T0 T  * 0  B − B  positivity condition θ&* ≥ 0 Solve the LP and perform sensitivity analysis as before.

231


3.3.5.1

Two Storey Frame With Concentrated Loading

232


233


3.3.5.2

Three Storey Frame With Distributed Load

An unbraced and rigid-jointed frame fabricated from S275 steel with pinned bases is shown. An investigation of the possibility of elasto-plastic instability is to be carried out to establish what load factor, applied to the given load would be required to cause such a failure.

The equilibrium equations are

234


And the Sensitivity Report,

235


The collapse load factor λPmin is 1.514 The basic variables as of the final tableau are those with finite allowable increase in the cost coefficient MP +

θ10

+

θ13

+

θ15

+

θ24

+

θ39

0

0.001738488 θ1 0.000977899 -θ14

0.000977899

0.001738488

-

0.000977899

-

0 θ28 0.000760588 0 θ40 0 θ27 Conversely, a non-basic variable is one with an infinite allowable increase in the cost coefficient MP. Amongst these, a potential basic variable is one with also a zero reduced cost. Here there is not any. Hence, there cannot be an alternate collapse mechanism, and the one predicted is unique. +

A unique bending moment distribution is obtainable if and only if there are α*+1 active participating hinges. Here, α*+1 = 10, and the number of active participating hinges is 6 from above. Hence, the exact bending moment distribution at collapse is not unique and is indeterminate. Plastic collapse load factor, λP =

1.51

236


3.3.5.3

Multi-Bay Portal Frame

237


238


3.3.5.4

Vierendeel Truss

239


3.3.6

Hand Methods Verification

3.3.6.1

Plastic Collapse Analysis by Solving Equilibrium Equations

The linear programming simplex method described above performs the plastic collapse analysis meeting the fundamental theoretical requirements as follows (i) The equilibrium equation is employed, hence satisfying the equilibrium condition (ii) Many different collapse mechanisms is postulated, hence satisfying the mechanism condition, and a linear solving algorithm is used to find the smallest λ (iii) The yield condition is automatically met since λ is minimized assuming that the chosen critical sections contains the critical mechanism. The hand method of plastic collapse analysis for simple structures of low degrees of static indeterminacies and a small number of critical sections is as follows (i) The equilibrium equation is employed, hence satisfying the equilibrium condition (ii) A collapse mechanism is postulated i.e. values and signs of the assumed bending moments MP is put into the bending moment at collapse {m} vector, hence satisfying the mechanism condition, and λ is solved for. (iii) Then {m} is computed and it is ensured that at no point of the structure, the bending moment is greater than the local MP value, hence satisfying the yield condition. Hence, naturally the smallest λ is found. Given simple frame with beam 2MP and columns MP subject to vertical 4λ and horizontal 1λ loading as shown. The plastic collapse load factor is required. 4λ 3

2

λ

4 α=2 C=4

L 1 2L

Appreciate that to form a mechanism we need α + 1 plastic hinges. Postulate Mechanism Condition with hinges at 1, 3 and 4. 4λ 3

2

λ

4

1 Formulate the equilibrium conditions noting the sign convention for positive bending moments and rotations. For bending moments, tension is positive and for rotations, extension is positive. 4λ 0

P2

-0.5 1

0.5

1

λ

-1.5

0

1 1

0

0

P1 P1=1 diagram

P2=1 diagram 240

λ=1/L diagram

-2.5


The Equilibrium Conditions are then 1 − M P   1   M   2 = 2  2M P   0    1 − − M P   2

p  m C = [B b 0 ]  α  λ Sign convention for extension positive

0  3 1 −   p1  2 p  1 0  2 5  λ L  1 −   2 0

Sign convention for tension positive

Solve the equations simultaneously. (1): p1 = −MP (3): p2 = 2MP (4): −MP = −0.5(−MP) + 2MP –2.5λL thus, λ = 1.4MP/L (2): M2 = 0.5(−MP) + 2MP – 1.5(1.4MP/L)L = −0.6MP Check that everywhere M ≤ MP. Here, OK. Thus Yield Condition met. Since mechanism condition, equilibrium condition and yield condition attained, the Uniqueness Theorem achieved. Note that we only need a load-equilibrating BMD (that not necessarily satisfies compatibility) for the external load whilst the BMD for the releases should satisfy compatibility. Let us try a different load-equilibrating diagram that DOES NOT satisfy compatibility, say pinned beams and cantilever columns. Postulate the same mechanism. 4λ  MP   1  M   0.5  2 =  2M P   0    − M P  − 0.5

0 − 1  p1  1 0    p2 1 2     λL  1 0  

λ

0

0 2

1

Solving these equations simultaneously will again result in λ = 1.4MP/L. But now, p1 = 0.4MP and p2 = −0.8MP. The values of p1 and p2 are no longer physically meaningful. Before it used to be the values of the indeterminate forces, now it is meaningless because of the non-compatible load-equilibrating BMD. An example design of a portal frame with haunches is presented.

241


242


243


3.3.6.2

Plastic Collapse Analysis by Virtual Work (Hobbs)

244


245


3.3.6.3

Plastic Collapse Analysis by Virtual Work (Chryssanthopoulos)

246


247


248


249


250


251


252


253


254


255


256


257


258


259


260


261


3.4 3.4.1

GNL, MNL, Contact Nonlinear Static and Buckling Analysis by The Implicit Tracing The Equilibrium Path Method Mathematical Formulation of Tracing the Equilibrium Path λ

ML, GL Static Analysis ML, GL Buckling Analysis λECR ML, GL P-∆ Static Analysis ML, GNL Static and Buckling Analysis (Tracing Equilibrium Path or Implicit or Explicit Time Integration with Dynamic Relaxation) MNL, GL Plastic Collapse Analysis λP



It is instructive to define a few important terms.

Definition of Equilibrium States and Paths

Equilibrium state

A pair of (λ,{U}) satisfying the geometrically nonlinear equilibrium conditions between the external nodal {P} loads and the component forces {f}, given the compatibility relationship between {d} and {U} as well as the constitutive law relating {f} to {d}

Equilibrium path

A continuous line of equilibrium states

Fundamental equilibrium path

An equilibrium path that includes the initial unloaded state (λ=0, {U}={0})

Secondary equilibrium path

An equilibrium path that does not include the initial unloaded state (λ=0, {U}={0})

Trivial fundamental path

An equilibrium path for which the displacements are zero for all levels of loading i.e. (λ≠0,{U}={0})

262


The static equilibrium equation has been established, and is restated in all its simplicity.

[K T ]δ{U} = δ{P} where

[K T ] = [K E ] + [K G ] T where [K E ] = [T ] [[k E ]][T ] [k E ] = ∫ [B]T [D][B]dΩ for which Ω

and

 ∂2 d



[K G ] = [T]T [[k G ]][T] + 

{f }

 ∂{U}∂ U  ∂ ε

[k G ] = ∫ 

for which

Ω 



2

∂{d}∂ d

{{σ}n

and

{σ}n = [D][B]{d}

and

{f } = ∫Ω [B]T [D][B]dΩ {d} +

[

  ∂ 2 Wi   ∂ 2 Wn  + {σ}i − [ D]{ε}i }dΩ −  − λ      ∂{d}∂ d   ∂{d}∂ d 

] {∫ [B] {σ} dΩ}− {∫ [B] [D]{ε} dΩ}− {∫ [N] {b}dΩ} T

Ω

Τ

T

i

Ω

i

Ω

[KT] = tangent stiffness matrix [KE] = instantaneous stiffness of the system with modified geometry as [T] dependent upon {U} [KG] = geometric stiffness matrix [KT], [KE] and [KG] are all symmetric. As stated, we have omitted the second order variation of work due to the external nodal loadings {P} from the above tangent stiffness matrix expression, i.e.  ∂2W   ∂{P}  −  = −   ∂ U   ∂{U}∂ U 

 ∂W  {P} =    ∂{U}

as

This is because, as mentioned, the externally applied loads at the nodes are in commercial codes always workconjugate with the nodal DOFs {U}, failing which the above term must be incorporated. The second order variation of work due to loads applied on the finite elements is obviously still taken into account. In order to find the buckling load, we could in theory perform a nonlinear eigenvalue solution. The nonlinear eigenvalue problem is expressed as [KT]{φ}={0} The nontrivial solution is obtained by solving for the eigenvalue λ from det | [KT] | = 0 This is quite a complex solution scheme is thus is not usually attempted. As closed-form mathematical solutions of realistic multi-degree of freedom nonlinear eigenvalue problems are highly complex, incremental methods to establish the equilibrium path is used. The incremental procedures can correspond to an increment of displacement or an increment of loading, i.e. displacement control or load control. The incremental approach is normally started from the initial unloaded equilibrium state, in which case the fundamental path is traced. In the vicinity of bifurcation states, it is essential that small incremental steps be used so as to avoid a jump from the fundamental path to a different path.

263


Tracing the Nonlinear Equilibrium Path λ λi

{G}j

ESi Full Newton Raphson

∆λ {P}j

λi-1

{R}j

ESi-1

Ui-1

∆U

Ui

U

{G} j = current out-of-balance force {R} j = [T] T {f} = current resistance force {P} j ={∂W/∂{U}}= current external nodal loading The vector {f} includes the fixed end forces which are negative terms here. It is equivalent then to add those terms to the {P} vector and call it the equivalent nodal loading vector if we desire; however the mathematics will work out nevertheless as the fixed end forces are included within {f} as negative terms. Now, in order to trace the nonlinear load path, we formulate a set of linear equations valid over a small load or displacement step. [KT]δ{U} = δ{P} This is the linearized equilibrium equation valid as long as [KT] is approximately constant over the displacement or load step. We can also rewrite the above equation as [KT]δ{U} = −{G} where {G} is the out-of-balance force between the equivalent loads and the resistance forces. In this way, there will be no accumulation of error as the load steps are traced. To trace the nonlinear equilibrium path, we ascertain i successive equilibrium states Between two successive equilibrium states j iterations are performed, ∆{U}j is solved from [KT]∆{U}j= −{G}j where {G} j ={R} j -{P} j ∆{U}= ∆{U} + ∆{U}j The Full Newton-Raphson recalculates [KT] at every j whilst the Modified Newton Raphson uses initial [KT] at beginning of iteration i Next j until out-of-balance force {G} ≈ 0, hence equilibrium state Next i noting that change in out-of-balance force δ{G} ≈ 0 signifies a limit point.

264


Iterative Method

Description

Advantages

Disadvantages

Newton-Raphson

[KT] calculated at every iteration in inner loop

Less iterations

Many [KT]-1 required for inner loop

Modified Newton-Raphson

[KT] calculated once before an iteration in inner loop

More iterations

Only one [KT]-1 required for inner loop

The modified Newton-Raphson is efficient when there is no strain hardening or an unloading path is not required, otherwise the Newton-Raphson is required for convergence. We start with load control. Load control used for ascending portions of the equilibrium path. When close to a bifurcation point, load control is used with small steps. Then when close to a limit point, displacement control is used. Displacement control is also used for descending parts of the equilibrium path. Then, if we come to a limit point in the displacement sense, we revert to load control or use another displacement parameter.

3.4.2

Newton-Raphson Load Control, Displacement Control or Arc-Length Control Algorithm

Advancing Phase 1. Determine an increment (of load, displacement or arc length) to trace on the equilibrium path from ESi-1 to ESi 2. Determine an estimate of the tangent stiffness at ESi-1, KTi-1 3. Determine the predicted displacement increment to move forward by solving the equilibrium equations [KTi-1]∆{U}Pi-1 = −{G}i-1 4. Calculate the element resisting force {R}i-1 5. Calculate the unbalanced force {G}i-1 and check for convergence. If converged, i.e. {G} ≈ 0, then go to 1 with i = i +1. If not converged go to 6.

Iteration (or Correcting) Phase 6. Determine an estimate of the tangent stiffness at ESj ESj = ESi-1 then Modified Newton Raphson ESj = ESj then Full Newton Raphson 7. Determine displacement increment due to the unbalanced force [KTi-1]∆{U}Cj = −{G}j-1 for Modified Newton Raphson where j – 1 = i – 1 [KTj]∆{U}Cj = −{G}j-1 for Full Newton Raphson where j – 1 = i – 1 8. Calculate the element resisting force {R}j 9. Calculate the unbalanced force {G}j and check for convergence. If converged, i.e. {G} ≈ 0, then go to 1 with i = i + 1. If not converged go to 6 with j = j + 1. If divergence occurs, then go to 1 with trying a smaller load step. Note that no convergence can be achieved if the total applied load is greater than the buckling load. The Full Newton-Raphson procedure can be expensive and unnecessary when the solution is close to convergence.

265


3.4.3

Equilibrium Paths, Stability of Equilibrium Paths, Critical Points, Stability of Critical Points

Apart from the linear eigenvalue method (linear elastic buckling) and nonlinear tracing the equilibrium path, stability if an elastic system can be interpreted by means of the concept of minimum potential energy. An elastic system always tend to go to a state in which the total potential energy is at a minimum. The types of instability include: (I)

Bifurcation instability (For perfect systems – SOL 105) (i) (ii) (iii)

(II)

Stable symmetric bifurcation Unstable symmetric bifurcation Asymmetric bifurcation

Limit load instability (For imperfect systems – SOL 106)

Bifurcation instability can be analyzed using linear buckling analysis whilst limit load instability is analyzed by tracing the equilibrium path. Load Stable symmetric bifurcation Unstable symmetric bifurcation Asymmetric bifurcation Limit load instability Deflection The energy method of stability analysis involves the following: (i) (ii)

Obtain the total potential energy function V = U – P∆ Obtain the equilibrium paths by solving for

∂V =0 ∂θ

(iii)

where for a SDOF system, a perfect system yields 2 solutions, one θ = 0 and the other P in terms of θ whilst an imperfect system gives one solution for P in terms of θ. Investigate the stability of the equilibrium paths ∂2V >0 ∂θ 2 ∂2V <0 ∂θ 2

(iv)

for regions of stability for regions of instability

Identify the critical points (i.e. the boundaries between stability and instability – bifurcation or limit points). For the perfect system, the critical point is the bifurcation point. This is obtain by inspection θ = 0, P = Pcr. Alternatively, the two solutions of (ii) is put into

∂2V =0 ∂θ 2 266


(v)

separately to yield two values defining the bifurcation point. We can also identify the limits points for imperfect systems by differentiating the equilibrium path equation, i.e. dP/dθ = 0. Hence we shall obtain value for θ at the limit point, θlp which subsequently is replaced into P for the value of the critical point, Plp. Investigate the stability of the critical point. The bifurcation point (θ = 0, P = Pcr) or the limit point (θ = θlp, P = Plp) is replaced into the third derivative of V. Unstable

∂ 3V

≠0

∂θ 3 =0

Unstable

<0

∂ 4V ∂θ 4

>0

Stable

=0 Repeat with higher derivative =0 Neutral stability Increment of total potential energy, ∆V = δV + δ 2 V + ... For equilibrium δV = 0 (principle of minimum potential energy), Increment of total potential energy around equilibrium state, ∆V = δ 2 V + ... =

1 ∂2V T δ{U}  2  ∂{U}∂ U

  δ{U} + ... 

=

1 T δ{U} [K T ]δ{U} + ... 2

An equilibrium state is stable if ∆V is positive for all possible infinitesimal disturbances δ{U}. This implies that an agent external to the system will have to perform positive work in order to cause δ{U}. Stability of Equilibrium State ES δ2V positive definite

Thoroughly stable ES

Gaussian elimination on [KT] leads to all positive diagonals, i.e. δ2V = 0.5 δ{U}T[KT]δ{U} > 0 for all δ{U} or det ([KT]) > 0

δ2V admits negative values

Thoroughly unstable ES

Gaussian elimination leads to at least one negative diagonal term, i.e. δ2V = 0.5 δ{U}T[KT]δ{U} < 0 for some δ{U} = δ{U0} or det ([KT]) < 0

267


δ2V positive semi-definite

Critically stable or unstable ES i.e. a critical point

Gaussian elimination leads to at least one zero diagonal term, i.e. δ2V = 0.5 δ{U}T[KT]δ{U} = 0 for some δ{U} = δ{U0} or det ([KT]) = 0

A critical point (buckling point) can be a bifurcation or a limit point. At a critical point det ([KT]) = 0, i.e. KT is singular indicating the presence of an infinitesimally adjacent equilibrium state at the same level of loading. A critical point is normally associated with one buckling mode δ{U0}. Bifurcation points are very rare in real structures due to the presence of imperfections in the geometry and due to pre-buckling displacements. Nature of Critical Point

Bifurcation point

A critical point is a bifurcation point if and only if the first order work done by {Pn} over the buckling mode(s) δ{U0} is zero. Loading can be increased further along at least one of the bifurcation paths.

{Pn}Tδ{U0} = 0

Limit point

A critical point is a limit point if and only if the first order work done by {Pn} over the buckling mode(s) δ{U0} is non-zero. Loading cannot be increased further.

{Pn}Tδ{U0} ≠ 0

268


3.4.4

MSC.NASTRAN Decks

3.4.4.1

GNL, MNL Load Control, Displacement Control or Arc-Length Control Static Analysis

All cards applicable to SOL 101 are also applicable to SOL 106. $ EXECUTIVE CONTROL SECTION SOL 106 $ CASE CONTROL SECTION DISPLACEMENT() = ALL/ SPCFORCES() = ALL/ OLOAD() = ALL/ NLSTRESS = () = ALL/ ELSTRESS() = ALL/ ELFORCE() = ALL/ STRAIN() = ALL/ ESE() = ALL/ BOUTPUT = ALL $ Slideline Contact Output Request $ SUBCASE 1 LOAD = < ID of FORCEi, MOMENTi, PLOADi, GRAV, LOAD, SPCD Cards in Bulk Data > TEMP(LOAD) = < ID of TEMP, TEMPRB, TEMPP1 Cards in Bulk Data > SPC = < ID of SPC Cards in Bulk Data > NLPARM = < ID in Bulk Data NLPARM > $ SUBCASE 2 LOAD = < ID of FORCEi, MOMENTi, PLOADi, GRAV, LOAD, SPCD Cards in Bulk Data > TEMP(LOAD) = < ID of TEMP, TEMPRB, TEMPP1 Cards in Bulk Data > SPC = < ID of SPC Cards in Bulk Data > NLPARM = < ID in Bulk Data NLPARM > $ BULK DATA PARAM, PARAM, PARAM, PARAM, PARAM, NLPARM

AUTOSPC, NO FOLLOWK, YES LGDISP, 1 LANGLE, 2 K6ROT, 100 ID

NINC (<1000)

EPSU

EPSP

$ $ $ $ $

AUTOSPC NO By Default Includes Follower Force Stiffness Includes Large Displacement Effects i.e. [T] not constant Rotation Vector Approach for Large Rotations Shell normal rotation restrained in nonlinear analysis Incremental KMETHOD KSTEP MAXITER CONV INTOUT Time For Creep, DT EPSW

MAXDIV

MAXBIS

MAXQN MAXR

MAXLS

FSTRESS

LSTOL

RTOLB

Unlike linear analyses schemes, nonlinear analysis schemes (SOL 106 and SOL 129) employ subcases on an incremental basis, instead of separate load cases and boundary conditions. In linear analysis, subcases represent an independent loading condition. Each subcase is distinct from each other. Nonlinear static analysis permits only one independent loading condition per run. For SOL 106, the bulk data loads and prescribed displacements are measured from the initial configuration. Hence latter subcases should refer to different load cards that have magnitudes that include the magnitude of load cards from previous subcases. Hence, if the same point is being loaded or displaced in a subsequent subcase, the load or displacement value referred by the subsequent subcase should be relative to the initial undeflected value of zero and not that of the previous subcase. Subcases are hence

269


cumulative. Loads and boundary conditions at the end of a subcase are the initial conditions for the next subcase. Hence if the load description is inadvertently omitted in subsequent subcases, the load will automatically be removed in an incremental fashion. Only one independent loading history can be applied during an analysis. In general, a different loading sequence requires a complete new analysis. The load to be applied during a particular stage (i.e. subcase) is referred to by the LOAD Case Control Command. NINC in the NLPARM bulk data entry is an integer that specifies the number of increments in the particular subcase, by default 10. The more linear the problem is, the smaller the value of NINC that can be acceptable. But when nonlinearity is significant such as at the onset of plasticity, at regions of stress concentration where each load step causes high stress changes, at contact regions with high forces and at the onset of buckling, the incremental load should be small (i.e. NINC must be large). Hence different subcases should be used to model different regions along the load path. Where nonlinearity of stiffness is small, NINC can be small, and when nonlinearity is large, NINC must be large. The load specified in a particular subcase minus the load specified in the preceding subcase is equally divided by NINC to obtain the incremental load for the particular subcase. Clearly, if convergence is a problem, this incremental load should be made smaller (by increasing NINC and/or decreasing the magnitude of load specified in the particular subcase relative to the previous subcase) until convergence. Self-weight and/or prestressed elements must be simulated by incorporating an initial load case followed by whatever static loading load case. Each subcase should not have NINC exceeding 1000 to control the database size, output size and restarts. The following can be performed with multiple subcases: (i) Loads can be changed, naturally (ii) Boundary conditions, i.e. SPC can be changed (iii) Solution strategy in NLPARM The follower force is calculated and incorporated by the use of PARAM, FOLLOWK, YES. We know how the prestress affects the differential stiffness, namely a tensile prestress causing an increase in stiffness. The effect of the follower force on the stiffness is different. For example, for a cylinder under external pressure critical buckling load may be over-estimated (even though the mode shapes are similar) in a SOL 105 and the natural frequencies in vibration may be under-estimated (even though the mode shapes are similar) in a SOL 103 in the absence of follower stiffness. To the contrary, these observations are reversed in case of centrifugal loads. Centrifugal forces as a constant (static) load are applied by a Bulk Data RFORCE to any elements that have masses. The follower stiffness due to centrifugal load has the effect of lowering stiffness (although the centrifugal load tensioning effect increases stiffness), consequently lowering natural frequencies (even though the mode shapes are similar) in a SOL 103 and lowering the buckling loads (even though the mode shapes are similar) in a SOL 105. This effect increases as the RPM increases, and it becomes significant when the RPM is over 1000. For moderately geometric nonlinear analysis, exclusion of follower stiffness affects the rate of convergence, but the converged solution is correct. For severely geometric nonlinear analysis, it may not be possible to obtain a converged solution without including follower stiffness. As the geometric nonlinearity intensifies, so is the effect of follower stiffness. Therefore, inclusion of follower stiffness greatly enhances the convergence if the deformation involves severe geometric nonlinearity. Output requests for each subcase are processed independently, but are appended after computation for output purposes. The INTOUT field is specified with YES, NO or ALL and determines whether the output is requested for each load increment within a subcase or just the last load step of the subcases. YES Output requested for every computed converged load increment within the subcases NO Output requested for only the last converged load increment of the subcases ALL Output requested for every computed and user specified load increment within the subcase INTOUT is especially important for restarts. For Newton’s iteration methods (i.e. without NLPCI) the option ALL is equivalent to YES but not when arc length methods (with NLPCI) are used.

3.4.4.1.1

Increment Methods (Load Control, Displacement Control or Arc-Length Method)

Load control is specified by having load card definitions. Naturally, the LOAD case control command is required. Load cards relevant to SOL 101 is also relevant to SOL 106 except for DEFORM cards. The applicable load cards are FORCEi, MOMENTi, PLOADi. GRAV, TEMP, SPC, SPCD etc. Loads which are stationary in direction throughout the analysis include: -

270


(i) FORCE, MOMENT, SLOAD (ii) PLOAD1 (iii) GRAV Loads which follow the motion of the grid or the element (i.e. follower forces that produce stiffness terms) include (i) FORCE1, FORCE2, MOMENT1, MOMENT2 (ii) PLOAD, PLOAD2, PLOAD4, PLOADX1 (iii) RFORCE (iv) TEMP, TEMPD, TEMPP1, TEMPP3, TEMPRB

Displacement control is specified by having SPCD card definitions, noting that grid points with displacements enforced by SPCD must also have an SPC entry. Note that enforced displacement can also be specified directly on the SPC bulk data entry, although this method is not recommended. Naturally, the LOAD case control command is required. Arc-length control is specified by having load card definitions and also a NLPCI card with the same ID as the NLPARM card. Arc-length control cannot be used in conjunction with displacement control SPCD cards. The arclength method is useful to trace unstable or post-buckling equilibrium paths defined by negative load control steps. The critical buckling load can be estimated by Newton’s load control method by performing the nonlinear static analysis until the solution cannot be obtained due to divergence, in which case the adaptive bisection method is activated in the vicinity of the critical buckling load and stops at the limit load close to the critical buckling load. But beyond that, the load control method does not work, and hence the arc-length method is required.

MAXR on the NLPARM card is the maximum ratio for the adjusted arc-length increment relative to the initial value, by default 20.0. The TYPE field on the NLPCI card could be CRIS (default), RIKS or MRIKS. 3.4.4.1.2

Stiffness Update Strategy (AUTO, SEMI or ITER using KSTEP)

The load is divided up into load steps. Each load step is then divided into iteration steps. KMETHOD specifies the method for controlling stiffness updates, whether AUTO (default), SEMI or ITER. With AUTO, NASTRAN automatically selects the most efficient strategy of when to update the tangent stiffness matrix based on convergence rates. The matrix could be updated in the middle of an iteration and will not be necessarily be updated at the beginning of the load step. AUTO is a good starting method. It essentially examines the solution convergence rate and uses the quasi-Newton, line search and/or bisection convergence acceleration methods to perform the solution as efficiently as possible without a stiffness matrix update. Highly nonlinear behaviour in some cases may not be handled effectively using AUTO. For AUTO (like SEMI), the stiffness matrix is updated on convergence if KSTEP is less than the number of iterations that was required for convergence with the current stiffness.

SEMI is similar to AUTO (it also uses the quasi-Newton, line search and/or bisection convergence acceleration methods) except that the tangent stiffness matrix will also be updated at the beginning of each load step, irrespective of the convergence status. Hence SEMI provides better convergence at the expense of higher cost. The SEMI method is an efficient method for nonlinear static iteration. For SEMI (like AUTO), the stiffness matrix is updated on convergence if KSTEP is less than the number of iterations that was required for convergence with the current stiffness. With ITER, the stiffness matrix is updated at every KSTEP iteration. KSTEP specifies the number of iterations before the stiffness update, 5 by default. It is a ‘brute force’ method. It can be most suited for highly nonlinear problems. Full Newton-Raphson is obtained by selecting KMETHOD = ITER and KSTEP = 1. Modified NewtonRaphson is obtained by selecting KMETHOD = ITER and KSTEP = MAXITER.

271


3.4.4.1.3

Convergence Acceleration Techniques (Quasi-Newton MAXQN, Line Search using MAXLS and LSTOL, Bisection using MAXITER, RTOLB, MAXBIS and MAXDIV)

The convergence acceleration techniques include quasi-Newton, line search and bisection. The stiffness updating schemes can be supplemented with quasi-Newton (QN) updates. MAXQN is the maximum number of quasi-Newton correction vectors to be saved on the database, equal to MAXITER by default. The BFGS update is performed if MAXQN > 0. The line search is controlled by MAXLS and LSTOL. MAXLS is the maximum number of linear searches allowed for each iteration, default 4. LSTOL requires a real number between 0.01 and 0.9 to specify the tolerance for the line search operation, default 0.5. The line search operation will be conducted if the error defining the divergence rate is greater than LSTOL. Computing cost for each line search is comparable to that of an iteration.

MAXITER specifies the limit on number of iterations for each load increment, 25 by default. If the solution does not converge at MAXITER iterations, the load increment is bisected and the analysis is repeated. Bisection is also activated if RTOLB, by default 20.0 is exceeded. RTOLB is the maximum value of incremental rotation (in degrees) allowed per iteration before bisection is activated. MAXBIS specifies the maximum number of bisections for each load increment, 5 by default. If MAXBIS is positive, the stiffness matrix is updated on the first divergence and the load increment is bisected on the second divergence. If MAXBIS is negative, the load increment is bisected every time the solution diverges until the limit on bisection is reached. If |MAXBIS| has been attained and the solution still has not converged then the value on MAXDIV, which specifies the divergence criteria for an iteration, 3 by default, is considered. If MAXDIV is positive, the best attainable solution is computed and the analysis is continued to next load increment. If MAXDIV is negative, the analysis is terminated. Hence, if we want the analysis to terminate if convergence has not been achieved, MAXDIV must be negative, not the default value. The recommended value for MAXDIV is thus −3. 3.4.4.1.4

Convergence Criteria (CONV, EPSU, EPSP, EPSW)

The convergence test is performed at every iteration. CONV specifies the flags to select convergence criteria, UPW or any combination, note default PW. EPSU is the error tolerance for displacement error (U) convergence criteria. EPSP is the error tolerance for load equilibrium error (P) convergence criteria. EPSW is the error tolerance for work error (W) convergence criteria. If displacement control is used, then there is a need for tighter tolerances for convergence. There is a facility to provide a default value depending on the type of analysis, type of elements and desired accuracy by specifying the NLTOL parameter and leaving the CONV, EPSU, EPSP and EPSW fields in the NLPARM blank. Models with gap, contact or heat transfer elements will have tighter default convergences. $ BULK DATA PARAM, NLTOL, ITOL

ITOL is an integer designating the level of tolerance as 0 (very high) 1 (high) 2 (engineering design) 3 (preliminary design) Default convergence tolerances are as follows.

NLTOL

Designation

0

Very High

No Gaps, Contact or Heat Transfer Elements EPSP=1.0E-3 EPSW=1.0E-7

With Gaps or Contact Elements EPSP=1.0E-3 EPSW=1.0E-7

272

With Heat Transfer EPSP=1.0E-3 EPSW=1.0E-7


(Default) 1

High

2

Engineering

3

Preliminary

EPSP=1.0E-2 EPSW=1.0E-3 EPSP=1.0E-2 EPSW=1.0E-2 (Default) EPSP=1.0E-1 EPSW=1.0E-1

EPSP=1.0E-3 EPSW=1.0E-5 (Default)

The quality of the mesh is essential in nonlinear analysis. Artificial stress concentrations due to poor modelling such as when beams interface with a shell mesh without special handling techniques will cause convergence difficulty. The mesh should also be adequately fine for good stress recovery, hence a h-element convergence exercise must be undertaken. This could probably be performed by repetitive linear analysis, the resulting converged mesh can be used with confidence in a nonlinear analysis. Other steps that can be taken to improve convergence are increase the number of load increments, break applied load into multiple subcases, use a more general material stress-strain definition instead of a bilinear model, avoid poorly shaped elements in regions of high stresses and introduce initial load steps in the solution to establish equilibrium in the model prior to increasing the nonlinearity. Contact regions should have a fine mesh in order to capture the contact stresses. If large deformations are expected to distort elements such that their accuracy may be called into question, it may be worthwhile to manually distort the elements in the opposite direction somewhat before starting the solution so that the final shape will be closer to the ideal shape.

3.4.4.1.5

Nonlinear Finite Elements in MSC.NASTRAN

Damping

Stiffness

Geometric Nonlinearity i.e. [T] Not Constant With {U}

Differential Stiffness i.e. From Element Force and Work Done

Large Strain Effect Hyperelastic i.e. [B] Not Constant With {d}

Material Nonlinearity i.e. [D] Not Constant With {ε}

CBAR PBAR MAT1 (MATT1) CBUSH PBUSH and PBUSHT CBUSH1D PBUSH1D CROD PROD MAT1 (MATT1), MATS1 CONROD MAT1 (MATT1) CTUBE PTUBE MAT1 (MATT1) CBEAM PBEAM MAT1 (MATT1), MATS1 CQUAD4, CTRIA3

Mass

Element

Nature of Nonlinearity of Stiffness

Yes

No

Yes

No

Yes

No

No

No

Yes

Yes

No

No

No

Yes

Yes

Yes

Yes

Yes

Yes

No

Yes

Yes

No

Yes

Yes

Yes

No

Yes

Yes

No

Yes

Yes

Yes

No

Yes

Yes

No

Yes

Yes

Yes

No

Yes

Yes

No

Yes

Yes

Yes

No

Yes

Yes

No

Yes

Yes

Yes

No

Yes

273


PSHELL MAT1 (MATT1), MAT2 (MATT2), MAT8, MATS1, CREEP CQUAD8, CTRIA6 PSHELL MAT1 (MATT1), MAT2 CQUAD4, CTRIA3 PLPLANE MATHP CQUAD8, CTRIA6 PLPLANE MATHP CHEXA, CPENTA, CTETRA PSOLID MAT1 (MATT1), MAT9 (MATT9), MATS1, CREEP CHEXA, CPENTA, CTETRA PLSOLID MATHP

Yes

No

Yes

No

Yes

No

No

Yes

No

Yes

Yes

Yes

Yes

Yes

Yes

No

Yes

No

Yes

Yes

No

Yes

No

Yes

Yes

Yes

No

Yes

Yes

No

Yes

Yes

Yes

Yes

Yes

Note that the CBAR element is not a nonlinear element i.e. its coordinates are not updated as the element deforms. The CBUSH is a generalized nonlinear spring - linear damper element. The CBUSH1D is a rod-type nonlinear spring - nonlinear damper element; it is a 1D version of the CBUSH element with added features. The CBUSH is NOT geometrically nonlinear, only materially. The CBUSH1D element can have geometric and material nonlinearity. The CBUSH1D element is the only element which can model rotation damping such as for modelling tuned pendulums mass dampers. The CROD, CONROD, CTUBE elements can be used to model cables as these elements are geometrically nonlinear, incorporates the differential stiffness and can refer to different stress-strain curves for tension and compression.

CGAP element can also be used to work in the opposite sense to a contact element in order to function as a cable element. That is to say, the element can be made to work only in tension by specifying a separation distance corresponding to the taut condition, above which the element is to be turned on and resist tension. The CBEAM element can model plastic hinges at its ends for plastic collapse analysis of frameworks. For this, the material type specified in the MATS1 card must be elastic-plastic (and perfectly plastic too) i.e. TYPE PLASTIC, and strictly not nonlinear elastic. The CBEAM is assumed to have its nonlinearity concentrated at its ends. Obviously if material nonlinearity is enabled, there can be no pin flags. The user need not specify the crosssection axis about which the yielding occurs, since the implementation allows for combinations of bending moments in two directions plus an axial load. The flexibility of the plastic hinge is based upon eight idealized rods at each end, chosen to match the total area, center of gravity and moments of inertia of the cross section. Note that rigid body elements RBEi, RBAR and RROD do not rotate in geometric nonlinear analysis i.e. their coordinates are not updated as the element deforms and hence are not nonlinear elements. Geometric stiffness is also not computed for rigid elements. Offsets are not recommended in nonlinear analysis, or even linearized buckling analysis. Overly stiff elements, as replacements are also not recommended as they may cause problems with convergence (MAXRATIO exceeded). Too stiff will give you mathematical problems and too flexible will create too soft a connection. Thankfully what you might consider "very stiff" is numerically still likely to be OK. In number terms you want something that is maybe 1000X stiffer than the local structure. If you are still unsure try 2

274


runs, with one having a bar 10 times stiffer than the other. If the answers are similar then you know it is stiff enough. To estimate the stiffness of the structure at that point connecting the gap, use simple beam formulae such as 12EI/L3 or 3EI/L3 or alternatively, apply an arbitrary load and ascertain the displacement from a SOL 101 static analysis. Midside grids on solid elements are not allowed for nonlinear analysis.

3.4.4.1.6

Contact Nonlinearity

There are three primary types of contact elements, namely point-to-point contact gap elements (CGAP), line-toline or surface-to-surface slide line contact elements (BLSEG) and general arbitrary line-to-line or surfaceto-surface contact elements. The CGAP element is a point-to-point contact element. Its element coordinate system is defined depending on whether the end grids points are coincident or not. If coincident, the orientation is defined by using the coordinate system CID, which if unspecified would default to the basic system. If the grid points are not coincident, the orientation is defined using the element x-axis using defined by the GA to GB grid orientation and the v vector is defined using X1, X2, X3 or G0 entries. Note also that no stress singularity will be introduced here by connecting many 1D gap elements to the shell or solid mesh. This is because of the multiple 1D element. Had there been just one 1D element connected to a shell or solid mesh, then certainly there will be stress singularity.

The two basic properties of the CGAP element are its initial gap and its compressive stiffness. If the initial nodeto-node separation becomes more positive, the gap has no stiffness and is for all intents and purposes dormant. As the separation becomes less positive and approaches zero or some predefined initial gap, the element wakes up and becomes a stiff spring, which resists further closure. The point at which the gap begins to resist this displacement is defined by the initial gap. This initial gap may be zero but the length of the element may not. The length of the gaps may be zero for solid elements by may not for shell elements, whereby the user may decide that due to mid-plane modelling, these two plates that might rest on each other, would by definition, be separated by half the sum of their thicknesses. By bridging this separation with gap elements assigned with initial gap of zero, the code will know that this initial position represents the two parts already in contact.

The orientation is of the CGAP (whether coincident or not) is important to define the direction of opening and closing as depicted in the figures below. Hence GA and GB must be attached to the correct portions of the model in order to simulate the correct opening and closing behaviour.

The preload F0 is useful to model friction because the frictional force is a function of the total compressive force which in turn is a function of the preload. Hence in a SOL 129 analysis, if the only contribution of gravity is to add

275


a normal force which would result in frictional forces, the normal forces induced in the contact elements can be specified as preloads instead of modelling the gravity load case explicitly.

Gap element stiffness controls the numerical stability. The compressive stiffness must simulate the local stiffness of the elements in the contact pair. If the stiffness is too high, the element may bounce as the load is incremented near zero separation. The closed gap stiffness should not exceed the adjacent DOF stiffness by 1000 times. If the stiffness is too low, external forces may actually drive one node through the other. The CGAP element should be used when there is very little relative displacement or sliding normal to direction of closure is expected. The process of choosing a gap stiffness may be an iterative one as an initially soft gap if stiffened to the point where penetration is minimal but the nonlinear solution still converges. Alternatively, the adaptive gap stiffness technology adjusts the gap stiffness internally to achieve convergence without penetration within some predefined tolerance. In the adaptive solution, the method of specifying the initial gap stiffness is the opposite of the manual iterative process. Choose a stiffer gap and let the code soften it as is required numerically. The adaptive method is clearly more efficient. Note that the mesh on either contacting surfaces should correspond exactly so that the gap elements are well aligned. Relative slide should be insignificant as this can cause the gap element to go into tension when in reality it is still in contact. This problem arises if the force in the gap element acts in the direction of the element. A better method would then certainly be to define the stiffness of the gap element in a particular DOF only i.e. normal to the contact interface. The gap element provides point-to-point contact. When the gap element is open, there is no contact and no friction. When the gap element is closed, there are three different conditions. The first case is when the gap is sliding (no friction). The second case occurs when the gap element is sticking (static friction). The third case occurs when the gap element is slipping (kinetic friction). Sometimes, it may be difficult to converge because of the switching among these conditions. Typical coefficients of friction are presented.

Material Contact Steel on steel (dry) Steel on steel (greasy) Brake lining on cast iron Rubber on steel Tire on pavement (dry) Wood on wood

Coefficient of Friction 0.3 0.05 to 0.1 0.3 to 0.4 1.0 0.8 to 0.9 0.2

On the PGAP Bulk Data entry, U0 and F0 are the initial gap opening and the preload, respectively. U0 is the separation of the gap element. If you are unsure about what preload to use, use the default value of zero. KA, KB, and KT are called the penalty values. KA is the axial stiffness when the gap is closed, KB is the axial stiffness when the gap is open, and the KT is the transverse gap stiffness. All you need to input is the KA value. KB is defaulted to be zero, and KT is defaulted as a function of KA. The selection of KA or a penalty value is critical to the convergence of the problem. The non-adaptive gap does not update this KA value. The new adaptive gap updates this KA value if you specify a positive value for TMAX. The default option for the new adaptive gap is NO adaptive stiffness update. This is when the TMAX value is equal to 0.0. If TMAX is a negative number, then MSC.Nastran uses the non-adaptive gap formulation. A good initial KA selection is roughly 1000 times the Young's modulus of the material that is in the neighborhood of the gap element. Fields 8 and 9 also require some

276


explanation. For the new adaptive value this is MU1, which is the static coefficient of friction, and MU2, which is the dynamic coefficient of friction. The non-adaptive gap elements use MUY and MUZ in the same fields instead of MU1 and MU2 values. Therefore, to compare the results using adaptive and non-adaptive gap elements, set both of these entries to the same values. On most problems, you will not know how to estimate the penetration depth or field 2 on the continuation entry. Therefore, if you skip the continuation entry, the default new adaptive gap is obtained, which is everything adaptive except the KA update. The recommended allowable penetration of TMAX is 10 percent of the thickness for the shell element, and for the solid element it is roughly 1/10,000 of the characteristic length for the problem. A small positive value will turn on the adaptive stiffness update, which will then converge at a faster rate. The maximum adjustment ratio or MAR in field 3 of the continuation entry is used only for the penalty value adjustment of the adaptive gap element. The default value of 100 is sufficient for most problems. Further discussion of CGAP parameters is warranted. U0 is self explanatory - the initial open value of the gap. F0 any preload you want to apply - be careful if KB is the only thing preventing rigid body motion. KA - this is the source of most convergence problems due to gap elements. It can be calculated from the local stiffness of the structure at the GRIDs to which the gap are applied. If you can't do this by hand (usually the case), then run a linear static (SOL 101) analysis with U0 temporarily set greater than 0.0 (or remove the gap element from the model for this run, if possible); this is so the gap stiffness you have already defined at KA does not influence the local stiffness. Then apply a unit load to both GRIDs of the gap in the direction of the gap X axis. Run the analysis and recover the displacement of both GRIDs in the gap X direction. Now take 1000 times the inverse of the displacement at the gap GRIDs and use the smallest value of the two for the value of KA. Now 2 questions arise. First, if the value of displacement in the gap X direction recovered from this run is, say, 3.4211378E-02 then I calculate KA so KA = 1000 * 1/3.4211378E-02 = 2.923E+04. Do I have to use this EXACT value ? No. The analysis is only sensitive to orders of magnitude of the value of KA. In the above case, therefore, I would use KA=3E+4 as the initial KA value. Second, do I have to apply unit loads to EVERY gap GRID in the model (I may have many, many gaps) ? In general, no. Because I am looking for the order of magnitude of the stiffness for KA, it is only necessary to select one gap for each region where I judge the stiffness will be significantly different from other regions. That is to say, if the structure to which the gaps is attached is roughly the same stiffness no matter which gap GRIDs I select, then one gap will be enough to get a good KA value. Using engineering judgement, I can see if the structure will have significantly different stiffness in different areas of the model where gaps are connected. A value of 3E+04 will work just as well as 2E+04 or 4E+04 in the above example. KB - generally I leave this as default unless I have unusual situations such as a very large value of U0. To illustrate this, take the example of a gap that has an open value U0=1. I calculate the value of KA to be 2E+16. I leave KB blank, so the default value becomes KA*1E-14 = 200. Now I apply my loads and eventually during the analysis, the gap closes. The gap will have moved 1.; gap force = KB*1. = 200. This may be a significant load compared with the applied load. In this case, I would force KB to 0.1 or smaller to avoid large gap forces due to large axial displacements in the gap. KT - generally I leave this at default as it is tied to KA via MU1. MU1 and MU2 are self explanatory. Friction will generally have a significant effect on the cost of the analysis. TMAX, MAR and TRMIN are useful if the local stiffness of the structure changes significantly as a result of the nonlinear deformations. They allow the gap stiffness to be adjusted during solution, but only approximate values can be calculated for these. For most cases, if the structure's stiffness at the gap GRIDs will not change significantly, I would not use adaptive gaps. The extra iteration of two that maybe needed to get convergence will in general be quicker than reforming the stiffness to get a not much better value for KA. Only if I expect local stiffness to change significantly would I use TMAX > 0.0. If TMAX is set to 0.0 (the default), the gap-induced stiffness update, gap-induced bisection, and subincremental process are enabled, but the penalty values (KA, KB, KT) remain unchanged. If TMAX is set to a small positive value, this has all the features of the gap when TMAX=0.0, and also enables the adaptive penalty capability where the penalty values are adjusted according to changes in the stiffness of the surrounding structure. A value for TMAX is calculated by examining the structure to which the gaps are attached. If these are shell elements, then a value of 10% of the thickness of the elements should be used. For other elements, such as beam elements, then an equivalent thickness is used, such as the depth of the beam in the axial direction of the gap. If the structure is a massive solid, then the ideal value of TMAX is two or three orders of magnitude less than the elastic deformation of the solid. This is not always easy to estimate, so a value of 1 * 10E-4 of the characteristic length of the model can be used. That is, determine the largest dimension of the model and use 10E-4 of that value. If TMAX

277


is too small, the solution will frantically try to adjust the penalty values to update the stiffnesses. If TMAX is too large; no update will occur and convergence may be elusive. MAR sets the maximum allowable adjustment ratio for the penalty values and must be in the range 1.0 to 10E6. The upper and lower bounds of the adjusted penalty values are K/MAR and K*MAR, where K is KA or KT. TRMIN sets the lower bound for the allowable penetration and is a fraction of TMAX. It must be in the range 0.0 to 1.0. Penalty values are decreased if the penetration is less than the minimum allowable penetration which is calculated from TRMIN * TMAX. What is allowable ? Back to good 'ol engineering judgement.

Convergence is often a problem in highly nonlinear problems such as in GAP-like problems. This following approach is normally a lot faster and more reliable than accepting the default NLPARM entries. The problem with gap analysis is that the non-linearity is a very severe On/Off situation. This can cause problems where you get numerical "chatter" when a gap is not open or tightly closed. This chatter makes Nastran think it is not converging and causes the loads to be bisected. Bisection can be the worst thing to happen, as it reduces the load and can mean the chatter gets worse. This causes another bisection and before you know it you are applying tiny load increments. Also, to help whenever a gap opens or closes, we must update the stiffness matrix every iteration. Hence use the full Newton Raphson. Finally to make the gap closure definite, apply all the load in 1 or 2 steps rather than the default 10. So in summary use the following settings on NLPARM for a pure gap problem. 1) NINC=1 or 2; 2) Use Newton Raphson. KMETHOD=ITER, KSTEP=1; 3) Switch off Bisection MAXBIS=0. If convergence is a problem such as in highly nonlinear problems, then the TSTEP method can always be used with KSTEP=1 such that stiffness is updated at every time step, hence there is no issue of convergence, just like in explicit nonlinear transient analysis. However, the time step size must still be small for accuracy. The CGAP element is not a geometrically nonlinear element, it is a small displacement element, i.e. its coordinates are not updated as the element deforms. The orientation of the contact plane does not change during deflection.

The slide line contact elements BLSEG (with BCONP, BFRIC and BWIDTH) are essentially contact curves that allow significant relative sliding between the contacting parts. Slide lines can also be used to model contact between surfaces by proper definition of the slide lines. This is done when two or more corresponding slide lines are positioned on the contacting parts such that they remain relatively coplanar throughout model deformations. The same stiffness considerations as those for gap elements apply the estimation of the stiffness may be more complicated than for gap elements. Friction between the sliding interfaces may be incorporated. The friction coefficient for FEA contact element should not be assumed to have a direct correlation to the friction coefficients pulled from data sheets. A handy test setup involves a mass on an inclined board supported by a spring. K

U

µ=

W sin θ − KU W cos θ

W 278


General contact elements are conceptually the simplest but the most computationally intensive. Sets of elements define the contacting parts. The contact stiffness is usually derived from the material properties of the elements in the contact pair – typically the Young’s Modulus and in some codes the material damping. The contact and separation directions are determined from the normals or boundaries of the contacting elements. These contact entities provide the smoothest and most realistic pressure distribution but the computational price is heavy. 3.4.4.1.7

Material Nonlinearity

Material models can be elastic or inelastic (the latter exhibiting different unloading path to loading path and hence plastic strain linear or nonlinear (the latter exhibiting a variable Young’s Modulus with respect to strain) strain-rate dependent or dependent temperature dependent or independent isotropic, orthotropic or anisotropic (defining properties in the three orthogonal directions)

Inelastic, Nonlinear (Limited), Isotropic Material for Beams, Shells and Solids MATS1 (TYPE PLASTIC). This material model can be used with CBEAM elements (with dedicated plastic hinges at their ends) to perform plastic collapse analysis of beam frameworks. The elastic-plastic material model requires the definition of the yield stress. The elastic-plastic material model also requires definition of the yield criteria, i.e. the criteria checked to initiate yield, namely Tresca, Von Mises, Mohr-Coulomb or Drucker-Prager. The hardening rule must also be specified, either no hardening (i.e. perfectly plastic), isotropic hardening or kinematic hardening. The isotropic hardening model does not take the Bauschinger effect into account and hence the compressive yield always equals the tensile yield. The kinematic hardening model will take into account the Bauschinger effect i.e. the reduction in the compressive yield once tensile yield has occurred and a stress reversal happens. Elastic, Nonlinear (General), Isotropic Material for Beams, Shells and Solids MATS1 (TYPE NLELAST). The nonlinear material model requires the general definition of the stress-strain curve with a TABLES1 entry, i.e. the multi-linear stress-strain curve. To model a nonlinear elastic cable, a CROD element with the appropriate area (on a PROD card) can be defined together with a MAT1 and MATS1 card, both sharing the same ID. The MATS1 card references a TABLES1 card which defines the nonlinear stress-strain characteristics of the cable with three points, for instance (-1.0,0.0), (0.0,0.0) and (1.0,2.05E11) to define a steel tension only cable element. Hyperelastic Material MATHP. Hyperelastic materials such as rubber, silicone and other elastomer behave differently than standard engineering materials. Their strain displacement relationship is nonlinear even at small strains and they are nearly incompressible. The Poisson’s ratio of hyperelastic materials may exceed 0.50, whereas specifying a Poisson’s ratio of 0.50 or greater will result in failure using any other solution method. If the elements undergo large net displacements, it is prudent to define hyperelastic elements, otherwise non-equilibrium loading effects may occur with small strain elements. Because of the corotational formulation where a large deformation is split into element rigid body deformation and element net deformation, small strain elements can be used to model large total deformation, but not large net element deformations. A fine mesh will usually ensure that element net deformations are small. If element net rotations exceed 20 degrees or if the element stretches by more than 10-20%, then large strain (hyperelastic) elements should be used. Material properties are usually entered as Mooney-Rivlin constants (consisting of distortional deformation constants and volumetric deformation constants) or as a set of stress-strain curves (of force versus stretch for simple tension, compression, shear and volumetric compression). Temperature Dependent Linear Elastic Material MATT1 Temperature Dependent Anisotropic Elastic Material for Shell MATT2 and Solid Elements MATT9 Creep Material CREEP

279


3.4.4.2

Nonlinear Static and Linearized Eigenvalue Buckling Analysis

Buckling (i.e. instability) occurs when the tangent stiffness matrix becomes non-positive definite. To estimate the buckling load, the following methods can be used. I. A SOL 106 can be performed until a non-positive definite stiffness matrix is detected. The load steps can be reduced (by the adaptive bisection method) so the stage at which the tangent stiffness matrix becomes nonpositive definite can be ascertained with greater precision, hence approximating the buckling load. II. Another method is to use the arc-length method to trace the limit state and the post-buckling path. III. Another option is to perform linearized buckling analysis at various stages of the equilibrium path based on the tangent stiffness and differential stiffness at that stage, so-called the linearized buckling analysis based on a deflected configuration. Note that this is not the true theoretical nonlinear eigenvalue extraction analysis. However, since the tangent stiffness and the differential stiffness are based on the deflected configuration from a nonlinear static analysis, we shall refer to this buckling analysis as the nonlinear buckling analysis. The nonlinear buckling analysis computes a load factor based on the tangent stiffness matrix at not the initial undeflected configuration, but at a certain deflected position. The eigenvalue extraction method is the usual linear eigenvalue solution scheme. The nonlinear buckling solution is based on the extrapolation of two consecutive incremental solutions. The tangent stiffness matrix is proportional to the external loads, which implies that the critical load may be linearly extrapolated, i.e. Pcr = Pn + α ∆P The tangent stiffness matrix is proportional to the displacement increments, hence the critical displacements may be obtained by extrapolating from the current state, i.e. Ucr = Un + λ ∆U Since the tangent stiffness matrix is proportional to the displacement increments i.e. it changes linearly with displacements, the internal loads are a quadratic function of the displacements. NASTRAN uses two converged solution points to form the differential stiffness matrix. Hence the buckling solution tends to be more accurate when these consecutive incremental steps are closer to the buckling point. Since we do not know where the buckling point is until the analysis is performed, the nonlinear buckling analysis is performed by dividing the load into a number of subcases and performing the buckling analysis in multiple subcases based on the tangent stiffness matrix at the current point. Hence, the deck would look exactly the same as a nonlinear static analysis with the additional METHOD command in certain subcases referring to the EIGB (with SINV being the (i) recommended extraction method) (ii) PARAM, BUCKLE, 2 (iii) KSTEP = 1 in the NLPARM card to force the stiffness matrix to be updated at every solution step $ CASE CONTROL SECTION Subcase 1 LOAD = < … NLPARM = < METHOD = < Subcase 2 LOAD = < … NLPARM = < METHOD = < Subcase 3 LOAD = < … NLPARM = < METHOD = <

> … > ID of EIGB Card in Bulk Data > > … > ID of EIGB Card in Bulk Data > > … > ID of EIGB Card in Bulk Data >

280


$ BULK DATA PARAM, BUCKLE, 2 EIGB

$ Buckling Parameter to Activate Nonlinear Buckling Analysis

ID

To illustrate the nonlinear buckling analysis, if the first subcase has a load totaling 1000 and the second subcase 3000, i.e. an additional 2000. Say, the first subcase refers to a NLPARM entry with 5 increments (i.e. NINC = 5), hence the incremental load is 200. And say the second subcase refers to a NLPARM entry with 20 increments (i.e. NINC = 20), hence the incremental load is 2000/20 = 100. Performing a buckling analysis at the end of the first subcase (by having a METHOD command and PARAM, BUCKLE, 2) solves for α from which the critical buckling load can be calculated as Pcr = Pn + α ∆P = 1000 + 200α Likewise performing a buckling analysis at the end of the second subcase (by having a METHOD command and PARAM, BUCKLE, 2) solves for another α from which the critical buckling load can be calculated as Pcr = Pn + α ∆P = 3000 + 100α Evidently, a better estimate of the buckling load is attained when the equilibrium point from which buckling analysis is undertaken is close to the buckling point.

3.4.4.3

Nonlinear Static and Linear Eigenvalue Modal Dynamic Analysis

Linear modal analysis is performed on the nonlinear static solutions to include effects of prestress and other nonlinearities. The linear eigenvalue solution analysis is performed based on the tangent stiffness matrix at the end of the particular subcase or subcases where the METHOD statement appears. The deck would look exactly the same as a nonlinear static analysis with (i) the additional METHOD command in certain subcases referring to the bulk data EIGRL or EIGR entries to select the linear eigenvalue extraction method (ii) PARAM, NMLOOP, L with the loopid L of any positive value as this is not a restart $ BULK DATA PARAM, NMLOOP, L

$ Loopid L can be any positive integer as this is not a restart

281


3.4.4.4

Restart From Nonlinear Static Analysis SOL 106 Into Nonlinear Static Analysis SOL 106

Restarts are allowed from converged solutions. A LOOPID is created after each converged load increment in static analysis. The restart .dat file should contain all the information from the previous analysis with the addition of the following cards. $ FMS RESTART $ BULK DATA PARAM, LOOPID, L PARAM, SUBID, M

$ Specifies Converged Solution L to Start From $ Specifies the Subcase Sequence Number M to Start Into

SUBID is not the subcase ID but the subcase sequence number, which will be the subcase ID if the subcases have been incremented by 1 from 1. The SUBID value should be incremented by one from the last value printed in .f06. The LOOPID should be the last value stored for restart as printed in the .f06. On top of the above additional cards, additional cards which define the restart should be included. The Case Control Section should have the additional subcases starting with a subcase with the SUBID. The following changes are allowed in the model: (i) Additional applied loads, naturally (ii) Changes to the boundary conditions i.e. SPC may be removed (iii) Addition of direct input matrices (iv) Changes to the grid points (v) Changes to the element, i.e. linear elements may be added or deleted, but should be drastic as to cause large initial imbalance of loads; also elastic material properties MAT1 may be changed.

3.4.4.5

Restart From Nonlinear Static SOL 106 Into Linear Solution Schemes SOL 107 to SOL 112

It is imperative to realize that linear restarts are incremental values with respect to the preload, not total values. Hence, the total values are obtained simply by adding the linear restart values to that obtained from the converged nonlinear static solution. It is advised to have KSTEP = 1 so that the tangent stiffness matrix is computed at every solution step and to ensure that the linear restarts are based on the very latest tangent stiffness matrix. The deck should obviously refer to the linear analysis being performed and not SOL 106. $ FMS RESTART $ BULK DATA PARAM, NMLOOP, L

3.4.4.6

$ Load step id at the end of the subcase from the SOL 106 run

Implicit Nonlinear Static (and Dynamic Analysis) SOL 400

As described in Section 4.9.8.5.

3.4.4.7

Implicit Nonlinear Static (and Dynamic Analysis) SOL 600

As described in Section 4.9.8.6.

282


3.5 3.5.1

GNL, MNL Static and Buckling Analysis by Dynamic Relaxation Dynamic Relaxation of the Explicit Finite Difference Scheme Solving Newton’s Dynamic Equilibrium ODE (LS-DYNA) λ

ML, GL Static Analysis ML, GL Buckling Analysis λECR ML, GL P-∆ Static Analysis ML, GNL Static and Buckling Analysis (Tracing Equilibrium Path or Implicit or Explicit Time Integration with Dynamic Relaxation) MNL, GL Plastic Collapse Analysis λP



In dynamic relaxation analysis it is assumed that the loads are acting on the structure suddenly, so the structure is excited to vibrate around the equilibrium position and eventually come to rest on the equilibrium position. Within the solution scheme, it is similar to transient analysis except that (i) artificial viscous damping is applied at each time step (ii) mass scaling (artificial addition of mass) is employed Termination occurs when the static solution is reached. If there is no damping applied to the structure, the oscillation of the structure will go on forever. Therefore, artificial damping is required in the form of reducing the calculated velocities of all the nodes by a factor at each timestep to allow the vibration to come to rest, and converge to the static solution. Convergence is checked by a convergence parameter, C = current distortional kinetic energy / maximum distortional kinetic energy. Distortional kinetic energy = total kinetic energy − total mass * (mass averaged velocity)2 / 2. The distortional kinetic energy is the component of kinetic energy that is deforming or distorting the model. In theory, the distortional KE should be zero when a static solution is reached. C typically vary between 1E-3 (loose) and 1E-6 (tight). Loads and prescribed motions (such as displacements, velocities and accelerations) applied during the dynamic relaxation should always be ramped up from zero in order to reduce the oscillations. Instantaneously applied loads will induce over-excitation of higher modes, thus lengthening the time taken to converge and possibly introducing errors. In reality, the static loads are applied in an infinite time interval so as to not induce any dynamic effects. Hence, the load should be ramped up slowly (in a duration greater than the fundamental period) so as not to induce considerable dynamic effects. If there are non-linear materials in the model, load curves which ramp up suddenly could induce large dynamic amplifications that could cause the non-linear materials to yield, when in reality they should remain elastic in the application of static loads. If any part of the model is required to yield (i.e. become non-elastic) as part of the equilibrium position then great care needs to be taken. This is a path-sensitive solution and the deformation should progress in a monotonic fashion, otherwise the degree of yielding will be incorrect. If all the material models within the finite element model are linear elastic, then the static solution (by dynamic relaxation) is path independent. As with all nonlinear static solutions that are based on solving the dynamic equilibrium equations, the solution is only valid if it is path independent, which in theory is only applicable to models limited to linear material properties. In a

283


true pseudo-static solution, the loading, deflections and the plastic behaviour increase monotonically. But the dynamic relaxation solution scheme will probably yield a sufficiently accurate solution so long as the dynamic oscillations are small at every stage of the analysis such that the variations of displacement (and hence elemental strain) are small so that excess plasticity is not generated. Dynamic relaxation can thus be used in models with nonlinear materials, but the time of application of the forcing function should be gradual so that the inertial part of the dynamic equilibrium equation does not incorrectly cause large displacements to occur and incorrectly cause the nonlinear materials to yield. If this happens, the material yields due to the dynamic effects of the solution scheme and not due to the underlying static loading, the latter of which is perfectly acceptable. The matter is further complicated if the material model have unloading curves as well as the plastic regions. To avoid the undesirable dynamic effects, there should thus be many time steps between each load increment so that there is plenty of opportunity for the velocities and hence accelerations to be damped down. Recall that artificial damping is applied at each time step. The time over which the loads are ramped up should aim to gently accelerate the model deformation and is dependent on the model. The time should not be so short that the model does not have time to react, effectively making the loading instantaneous. However, the time should not be too long, which would increase the time taken to converge. This is because the convergence parameter is based on the initial to the current kinetic energies. If even the initial kinetic energy in the model is too small (as a result of too gently accelerating the model) then for a certain convergence ratio, the current kinetic energy will have to be much smaller. A duration slightly greater than the fundamental period is appropriate. As we are not interested in the dynamic response (since this is a static solution), the mass matrix can be artificially formed so as to maximize the time step which is limited by the lowest natural period in the model divided by π. Hence, mass scaling can be employed if damping is not sufficient to produce a converged static solution quickly. Mass scaling will also reduce the dynamic effects as the acceleration become smaller. To perform dynamic relaxation, two steps are undertaken (i) first, run the dynamic relaxation analysis with as little damping as possible. If c is the damping constant corresponding to the fundamental frequency, defining k = 1 − 2ζωndt let k = 0.9999999; this allows the model to oscillate, enabling its natural frequency to be determined. (ii) then, calculate the constant k corresponding an under-damped system k = 1 − 2ζωndt ζ = desired fraction of critical damping ωn = lowest natural frequency of oscillation (rad/s) dt = timestep effectively choosing a constant k that will result in the model being under-damped. Another method of applying the artificial viscous damping is using DAMPING_GLOBAL which applies global viscous damping proportional to the mass, i.e. damping force = c.v = 2ζmω.v = 2ζm2π/T.v = 4ζπ/T.m.v. The user specifies 4ζπ/T where T corresponds to the natural frequency of the most prominent mode excited by the excitation. Ideally, critical damping will provide the most efficient dynamic relaxation. However, experience has shown that it is usually better to under-damp the model. An under-damped model will move just past the equilibrium position and then rebound to converge on the correct solution. This process is relatively easy to monitor and the equilibrium position becomes obvious. However, a critically damped model will not rebound, since it moves directly to the equilibrium position, and thus can often look similar to an over-damped model. Experience shows that damping in the order of about 5% of critical is about optimum and not much higher. If the equilibrium position is path-sensitive (i.e. certain materials are required to yield), then ideally a critically damped model should be used. Alternatively, use plenty of time steps within each load increment so that the dynamic effects are very much reduced.

284


Ensure that all parts of the model have a velocity less than the terminal velocity. If parts of the model need to displace a relatively large distance before reaching equilibrium, then the model may reach terminal velocity. This is when the reduction in velocity due to relaxation damping just cancels out the increase in velocity due to loading (i.e. no resultant acceleration). This causes dynamic relaxation to take a long time because Vterminal limits the speed of deformation. To overcome this, ramp up the loading to greater than the real loading (2-3 times gravity) to deform faster, thus increasing Vterminal, then as equilibrium position reached, ramp load back down, ensuring no additional modes of deformation occurs that would not have occurred under normal magnitude loading. Vterminal = F * dt * k / (m*(1-k)) F = desired fraction of critical (normally 1.0) dt = timestep m = mass of body k = damping constant The effectiveness of the dynamic relaxation solution scheme is investigated by plotting the variation of the convergence parameter as shown below.

Convergence Parameter C

Time

(a) (b)

(c)

(d)

The most common problem with dynamic relaxations is that the solution fails to converge or appears to take too long to converge. Referring to the plot above, we can identify 4 cases (a) (b)

(c) (d)

Solutions that never start to converge or take too long to converge. This can be caused by severe over-damping or by an insufficiently resisted (but loaded) mode of deformation. Apply a lower damping constant during the dynamic relaxation phase Solutions that partly converge but never reach the convergence tolerance. This can be caused by hourglassing or high modes of oscillation such as single element modes. To solve these problems, try using a different hourglass control or significantly reduce the timestep by say a factor of 5 for the dynamic relaxation phase Severe under-damping The correct solution

285


3.5.2

LS-DYNA (GNL, MNL Explicit Transient) Dynamic Relaxation Cards

To specify termination time of zero for the explicit dynamic analysis to have no limit *CONTROL_TERMINATION Termination Termination Termination Change in Termination Min Time Termination Energy Ratio Total Mass Step Size Cycle Limit Time Limit Limit From Mass Limit Scaling To set structural timestep size control and invoke mass scaling if necessary *CONTROL_TIMESTEP Min Time Maximum Initial Time Factor For Shell Min Step For Basis Time Step Step Time Step Mass Time Step Curve Scaling

Erosion Flag

Limit Mass Scaling

To define controls for dynamic relaxation *CONTROL_DYNAMIC_RELAXATION To specify user-defined boundary conditions for the dynamic relaxation (stress initialization) phase, *LOAD_NODE_ (HM: forces, moments) *SET_NODE *DEFINE_CURVE with SIDR = 1 for stress initialization phase *LOAD_BEAM_ *SET_BEAM *DEFINE_CURVE with SIDR = 1 for stress initialization phase *LOAD_SHELL_ (HM: pressure ShellPres) *SET_SHELL *DEFINE_CURVE with SIDR = 1 for stress initialization phase *LOAD_RIGID_BODY *DEFINE_CURVE with SIDR = 1 for stress initialization phase *LOAD_SEGMENT_ (HM: pressure SegmentPre) *SET_SEGMENT *DEFINE_CURVE with SIDR = 1 for stress initialization phase To apply automatically computed gravitational loads, noting that by d-Alembert’s principle, applying accelerations in a certain direction results in inertial loads acting in the opposite direction, *LOAD_BODY_Z with sf = 9.81 ms-2 *DEFINE_CURVE with SIDR = 1 for stress initialization phase

286


To prescribe displacements boundary conditions on a node, on a set of nodes, on a rigid body in the global axes system or on a rigid body in the rigid body local axes system, *BOUNDARY_PRESCRIBED_MOTION_ Load Curve NID, NSID, Displacement VID DEATH DOF LCID Scale Factor or PART ID VAD SF The vector ID, VID is used to specify a direction vector if imposed motion not in global axes system. *SET_NODE_LIST DA1 NSID NID NID NID NID

DA2 NID NID

DA3 NID NID

DA4 NID …

NID …

NID …

*DEFINE_CURVE LCID SIDR Abscissa Values Abscissa Values …

SFA SFO Ordinate Values Ordinate Values …

OFFA

OFFO

DATTYP

BIRTH

NID …

SIDR defines whether the curve is valid for the transient phase, stress initialization phase or both. Here obviously, SIDR = 1. The curve should define a constant value of displacement valid throughout the analysis. If the dynamic relaxation phase is to be followed by a transient seismic analysis, it is necessary to define zero velocity prescribed boundary conditions for the dynamic relaxation phase on the nodes at which the transient accelerations are applied so that the structure is supported during dynamic relaxation. *DEFINE_VECTOR if DOF not global VID XTail YTail

ZTail

Xhead

287

Yhead

ZHead


4 METHODS OF DYNAMIC ANALYSES 4.1 GL, ML Implicit Real Modal (Eigenvalue) Analysis 4.1.1

Mathematical Formulation of Analysis

The natural frequencies of a structure are the frequencies at which the structure naturally tends to vibrate if subjected to a disturbance. Hence modal analysis warns if the dominant forcing frequencies are close to the lowest natural frequencies of the structure, indicating resonance behavior of the lowest modes of the structure. The equation of motion for a free, undamped system is [M ]{& u&( t )} + [K ]{u ( t )} = {0} We seek solutions of the form

[

{u(t)}i = Re al {φ}i ξ i e λ i t

] for the i

th

mode of vibration

where ξ i = ξ Ri + iξ Ii and λ i = α i + iω di . Note that α represents the decaying part and ω d the damped natural frequency. Hence, substituti ng into the equation of motion [M ]ξ i λ2i {φ}i e λ i t + [C]ξ i λ i {φ}i e λ i t + [K ]ξ i {φ}i e λ i t = {0}

[λ [M] + λ [C] + [K]]{φ} 2 i

i

i

Since there is no damping α i = 0 and ω di = ω ni Thus

[− ω

]

2 ni [ M ] + [ K ] {φ}i

= {0} and so λ i = iω ni

= {0}

This is a real eigenvalue problem to be solved for ω ni and {φ}i . For each mode i, NASTRAN outputs the modal frequency ω ni and the mode shape {φ}i . For completion, the response due to mode i, {u(t)}i of a free undamped linear elastic structure subjected to an initial impact (defining an initial displacement and velocity) is

[

{u(t)}i = {φ}i Re al ξ1i e λ1i t + ξ 2i e λ 2 i t

]

{u(t)}i = {φ}i Re al [(ξ1Ri + iξ1Ii )(cos ω ni t + i sin ω ni t ) + (ξ 2 Ri + iξ 2 Ii )(cos ω ni t − i sin ω ni t )]

{u(t)}i = {φ}i Re al [((ξ1Ri + ξ 2 R ) cos ω ni t − (ξ1Ii − ξ 2 Ii ) sin ω ni t ) + i((ξ1Ii + ξ 2 Ii ) cos ω ni t + (ξ1Ri − ξ 2 Ri ) sin ω ni t )] For the free vibration response to be real for all t, and ξ1Ii = −ξ 2 Ii ξ1Ri = ξ 2 Ri Since there are two less independent constants, let and ξ1Ii = −ξ 2 Ii = ξ Ii ξ1Ri = ξ 2 Ri = ξ Ri We notice that ξ1i and ξ 2i are a complex conjugate pair ξ1i = ξ Ri + iξ Ii and Hence

ξ 2i = ξ Ri − iξ Ii

{u(t)}i = {φ}i (2ξ Ri cos ω ni t − 2ξ Ii sin ω ni t )

Thus the total response due to the superposition of all modes {u(t)} = [Φ ]{(2ξ Ri cos ω ni t − 2ξ Ii sin ω ni t )}

288


Re writing the eigenvalue problem [[K ] − ωni [ M]]{φ}i = {0} as 2

[K ]{φ}i = ωni [M ]{φ}i 2

and premultiplying by{φi }

T

{φi }T [K ]{φ}i = ωni 2 {φi }T [M]{φ}i K i = ωni 2Mi hence, the i th generalized mass Mi = {φi } [M ]{φi } T

and the i th generalized stiffness K i = {φi } [K ]{φi } T

Note that the value of the generalized (or modal) mass and generalized (or modal) stiffness is arbitrary since it is dependent upon how the corresponding eigenvector has been normalized. However, for a particular mode,

K i = ω ni Mi 2

Also, the Rayleigh’s quotient is obtained as {φ }T [K ]{φi } K ω 2ni = i = i T Mi {φ i } [M ]{φi } Because the normal modes are independent of each other, the orthogonality condition holds.

&

{φi }T [M]{φ j } = 0 {φi }T [K ]{φ j } = 0 if i ≠ j

Hence, we can obtain the diagonal modal mass and the diagonal modal stiffness matrices. modal mass matrix, [M] = [Φ ] [M ][Φ ] T

[ ]

modal stiffness matrix, [K] = [Φ ] [K ][Φ ] = ω 2 [M] T

Again, the following relationship holds,

[K] = [ω2 ][M]

A normal modal analysis indicates the best location for the accelerometers in dynamic testing. Design changes can be evaluated with a normal modal analysis, in that if a particular modification were to cause a change in the frequencies and mode shapes, then the response in also likely to change. This is done with the knowledge that the natural frequencies are a function of the structural properties and boundary conditions but the mode shapes are a function of only the boundary conditions. Modal strain energy is a useful quantity in identifying candidate elements for design changes to eliminate problematic low frequencies. Elements with large values of strain energy in a mode indicate the location of large elastic deformation (energy). Stiffening these elements will increase the natural frequency more than stiffening other elements. It must be understood that the scaling (or normalization) of the normal modes are arbitrary, hence their do not indicate the response. This means that a different scaling method will yield a different modal (or generalized) mass, modal stiffness (but same modal frequency) and different modal response. However the response due to the particular mode in the physical coordinates will be unique irrespective of the method of scaling. Even the comparison of magnitude of response between the different mode shapes or different modal masses in itself to determine relative importance of each mode is incomplete (as the amplitude and location of the excitation i.e. the modal mass is also important), although the response on different parts of the structure due to a particular

289


mode can be indicative of the more stressed parts due to that particular mode. But it remains that the mode shapes only represent the shapes of vibration that the structure vibrates in, and not the magnitude, which is dependent upon the amplitude and location of loading and the relation between the forcing frequencies and the natural frequencies. Three methods of eigenvector scaling exists, namely (i) MASS normalization Ensures {φi}T[M]{φi} = 1.0. Saves computational effort and storage. However, for very heavy structures, [M] becomes large, and so {φi} can be very small. The magnitudes of the mode shapes of different modes cannot be compared to determine relative importance. The modal stiffness will be the square of the natural modal frequency because Ki = ωni2 Mi = ωni2(1) = ωni2. (ii) MAX normalization Scales the eigenvectors such that the maximum component is unity for each and every mode. Modal masses of the same order in themselves cannot be used to determine relative participation of individual modes (as the amplitude of the modal force is also of significance), however a small modal mass obtained from this normalization clearly indicates a local mode or an isolated mechanism. (iii) POINT normalization This allows the user to choose a specific displacement component at which the modal displacements are set to 1 or –1. Useful if user knows the maximum displacement location and component. However, this normalization is not always recommended because for complex structures, the chosen component may have very small values of displacement for higher modes causing larger numbers to be normalized by a small number, resulting in possible numerical roundoff errors and ridiculously higher modal masses. For instance, if the POINT normalization points to a DOF component which does not really exist in a particular mode, than all the other eigenvector terms will be normalized by a very small number, which will certainly result in numerical errors. In this method, the modal masses can be compared between modes if the DOF chosen for POINT normalization corresponds to the solitary point of load excitation, i.e. ensuring that the (amplitude of the) modal force is the same between different modes. In this case, the higher the modal mass, the lower will be the response. The orthogonality of normal modes signifies that no mode can be obtained from a linear combination of other modes. The representation of a normal mode by using a modal mass and modal stiffness is useful for formulating equivalent dynamic models and in component mode synthesis. Rayleigh’s quotient as presented above is analogous to the equation of natural circular frequency ωn2 = K/M for a SDOF system, here instead the natural circular frequency of the mode is the division of the modal stiffness to the modal mass, square rooted. Identical eigenvalues (repeated roots) occur in structures that have a plane of symmetry or that have multiple identical pieces (such as appendages). The eigenvectors (mode shapes) for these repeated roots are not unique because many sets of eigenvectors can be found that are normal to each other. Consequently, small changes in model or different computers can make large changes in the eigenvectors for the repeated roots. Rigid body modes are a special case of repeated roots. The modal dynamic analysis is based on only the instantaneous stiffness matrix at the initial undeflected stage. The modal dynamic P-∆ (KGA From KTA) analysis is based on the instantaneous and geometric (or differential) stiffness matrices at the initial undeflected stage i.e. taking in to account the effect of the initial prestress and initial nonwork conjugate external load on the stiffness of the structure in the computation of the structural frequencies and mode shapes. Modal Dynamic [[ K AE ] − ω ni [ M ]]{φ}i = {0} 2

Modal Dynamic P - Delta [[ K TA ] − ω ni 2 [ M ]]{φ}i = {0} It is worth noting that only the stiffness and the mass distribution of the structure determine its modes. The static equilibrium displacement does not come into the equations. However, if geometrical non-linearity is taken into

290


account, the tangent stiffness of the structure will change from the initial undeflected configuration to its static equilibrium configuration, in which case the real modal analysis will be affected. It is important to check for rigid body motion. The rigid body modes involve translation or rotation of the model, without any deformation i.e. stress free conditions indicating modelling errors is an inadequate constraint set or the analysis of unconstrained structures such as airplanes. Rigid body modes have a zero frequency. In practice, due to roundoff errors the frequency of these modes is a small number. The modes do not occur in such a pure form and are often coupled together in some way but there should always be 6 rigid-body modes and their natural frequencies should be close to 0.0 Hz (~1.0E-4) as their modal mass is greater than zero whilst their generalized stiffness is zero. The user should check that this number is several orders of magnitude lower than the lowest natural frequency. A zero frequency mode which does not also have zero strain energies is not a rigid body mode, instead could be a mechanism and as such should be investigated. The number of rigid body modes depends on the way the structure is supported. For example, an unsupported vehicle model would produce 6 rigid body modes (3 translations, 3 rotations), a model of half the vehicle with symmetry boundary conditions should produce 3 rigid body modes. A cantilever beam should have no rigid body modes. A common modelling error resulting in a mechanism is when a bar is cantilevered from a solid element; the bar has rotational stiffness and the solid has no rotational stiffness, resulting in a pinned connection when the two are joined. The user should check the natural frequency is of the right order of magnitude. For example, the lowest bending and torsion modes in a standard saloon vehicle are 20-30 Hz, while the lowest modes in multi-story buildings are 2-5 Hz. The natural modes should be animated, and the overall behavior should be assessed. It is important to distinguish between fundamental modes involving the whole structure, and local modes involving limited zones. The local modes can often be due to modelling problems (for example flapping panels in vehicle structures), and a judgment should be made whether they are unrealistic. Modal analysis is extremely useful to check for unrestrained degrees-of-freedom. Note that in this case the analysis will often run but spurious mode shapes will often result involving a component that has not been properly attached to the main structure. It is often true that merely by post-processing the results from a modal analysis and studying the mode shapes most of the problems concerning the connectivity of the FE model become apparent. Alternatively, the edges of the finite element mesh can also be highlighted with a preprocessor and this could provide useful insight. A matrix whose eigenvalues are all greater than zero is said to be positive definite. If the eigenvalues are zero and positive, the matrix is positive semi-definite. An unconstrained structure would have a positive semi-definite matrix. If all the rigid-body modes are constrained, the stiffness matrix will then be positive definite. An extremely reliable mathematical tool that determines the number of eigenvalues that exists within a certain frequency range is the Sturm Sequence Check. This is printed under UIM 5010 and should be inspected always. Modal testing and analysis correlation is done using orthogonality checking and Modal Assurance Criteria (MAC) using the postmaca.v2001 DMAP alter. It allows for the quick assessment of modal vectors obtained from test data. The orthogonality check indicates if a set of vectors is orthogonal to the mass matrix, and hence shows if the large mass terms have reasonable agreement between test and analysis. The MAC indicates a set of vectors is linearly independent, and hence indicates how well the modal vectors from the test and analysis agree with each other. As a general rule for the two checks, the diagonal terms should be greater than 0.9 (with lower order modes very close to unity) and off-diagonal terms should be less than 0.1. Note that both the analysis DOFs and test accelerometers should be in the same location and orientation.

Orthogonal ity Check Modal Assurance Criteria, MAC ij

[Φ ]Tt [M ][Φ ]a = [I ]

((φ ) (φ ) ) (φ φ ) (φ φ ) T t i

T t

t i

291

2

a

T a

j

a j


4.1.2 4.1.2.1

MSC.NASTRAN Decks GL, ML Real Modal Analysis

$ EXECUTIVE CONTROL SECTION SOL 103 $ CASE CONTROL SECTION $ Sets defining grid ids or element ids SET < Number > = 1 THRU 100, 211, 343, < etc > $ Grid output of displacement for each mode i.e. eigenvector $ SORT1 lists the results by eigenvalue whilst SORT2 lists the results by grid id DISPLACEMENT(,) = ALL/ $ Grid output of real eigenvector for the a-set SVECTOR() = ALL/ $ Grid output of SPC forces SPCFORCES(,) = ALL/ $ Element output of force, stress and strain ELFORCE(,) = ALL/ ELSTRESS(,) = ALL/ STRAIN(,) = ALL/ $ Analysis Cards SPC = < ID of SPC Cards Defined in Bulk Data > METHOD = < ID IN EIGRL or EIGR > $ XY plot output OUTPUT(XYPLOT) XYPUNCH RESPONSE /() XYPUNCH RESPONSE /() The recommended method of eigenvalue extraction is the Lanczos method, which combines the best characteristics of both the transformation (Givens, Householder, Modified Givens, Modified Householder) methods and iterative tracking (Inverse Power, Strum Modified Inverse Power) methods. The Lanczos method requires that the mass matrix be positive semi-definite and the stiffness be symmetric but does not miss modes. The Lanczos method is defined with an EIGRL entry which allows either MASS (default) or MAX eigenvector normalization. $ BULK DATA EIGRL ID Lower Frequency (Hz) Upper Frequency (Hz) Number of Eigenvalues MSGLVL MAXSET SHFSCL Eigenvector Normalization Method A backup method that does not miss roots and is useful for finding out the first few modes for very large models that do not fit in memory is the Sturm Modified Inverse Power Method (SINV), which allows either MASS (default), MAX or POINT eigenvector normalization. $ BULK DATA EIGR ID SINV Lower Frequency (Hz) Eigenvector Normalization Method Grid ID for POINT DOF for POINT Upper Frequency (Hz) 292 Number of Eigenvalues Structural Engineering Analysis and Design Second Edition 4.1.2.2 GL, ML P-∆ (KGA From KEA) Real Modal Analysis It is often necessary to incorporate the reduction in bending stiffness of gravity load resisting columns for the analysis of lateral loads. The following procedure is undertaken. Phase 1 Perform static analysis (with loads that cause the greatest negative or positive geometric stiffness) based on [KEA] but include the segyroa.v2001 alter prior to the Case Control Section in order to compute the geometric stiffness matrix [KGA]1 (and output into a .pch file) based on the generated element loads from the [KEA] static analysis. Phase 2 A SOL 103 is undertaken based on [KEA] + [KGA]1 with the k2gg=ktjj statement in the Case Control Section and the outputted .pch file which contains the ktjj matrix in the Bulk Data. The responses at this stage represent the P-∆ (KGA From KEA) real modal response. The following equivalent alternative procedure can also be employed. $ CASE CONTROL SECTION SUBCASE 1 LABEL = Static Preload Load Case LOAD = < ID of FORCEi, MOMENTi, PLOADi, GRAV, LOAD, SPCD Cards in Bulk Data > TEMP(LOAD) = < ID of TEMP, TEMPRB, TEMPP1 Cards in Bulk Data > DEFORM = < ID of DEFORM Cards in Bulk Data > SUBCASE 2 LABEL = P-∆ Modal Analysis STATSUB(PRELOAD) = 1 METHOD = < ID in EIGRL > The method is valid when only the prestress is judged to affect the geometric stiffness such as in the compressive preload of building columns due to gravitational loads and the prestressing of extremely taut cables that sag very little under gravity but not in systems such as suspension bridges. Where lateral loads are large enough to affect the geometry of the system with prestress, then a repetitive P-∆, SOL 106, implicit dynamic relaxation SOL 129 or explicit dynamic relaxation must be employed. But in single P-∆ analysis, because cables do not have much elastic bending stiffness, the initial static preload subcase should only include the prestress and not gravity as including gravity is the same as solving two linear static problems of stiffness KEA with preload and gravity as the applied loads respectively. Clearly, in the gravity case, it is nonsensical as the cables do in reality have differential stiffness (from the prestress) to resist the gravitational force. Prestress in one direction (i.e. along the axis of cable) will cause a differential stiffness in the orthogonal direction. Gravity acts in the orthogonal direction and hence cannot be accounted for in the calculation of the prestress in this single P-∆ analysis. To quantitatively decide if gravity need not be considered in contributing to the differential stiffness of the cables, a static P-∆ analysis should be carried out, the first subcase being a SOL 101 with only the prestress as applied loads and the second subcase a P-∆ SOL 101 (i.e. utilizing the induced prestress from the first subcase to form a geometric stiffness matrix) with both the gravity and prestress included as applied loads. If the difference in the cable element forces between subcases 1 and 2 is negligible, then gravity has little influence in affecting the geometric stiffness. If there is a major difference in the cable element force, then clearly, gravity will affect the geometric stiffness and as such, a repetitive P-∆ , SOL 106, implicit dynamic relaxation or explicit dynamic relaxation must be used to converge to the true KT. Likewise, in the single P-∆ analysis of multi-storey buildings, gravity (and only gravity) acts in axis of columns to generate prestress, and the differential stiffness is computed for the orthogonal direction reducing resistance to lateral wind forces, applied in the second subcase with gravity too. 293 Structural Engineering Analysis and Design Second Edition The STATSUB(PRELOAD) computes the differential stiffness due to the prestress and also the follower force. The follower force is calculated and incorporated by the use of PARAM, FOLLOWK, YES. We know how the prestress affects the differential stiffness, namely a tensile prestress causing an increase in stiffness. The effect of the follower force on the stiffness is different. For example, for a cylinder under external pressure critical buckling load may be overestimated (even though the mode shapes are similar) in a SOL 105 and the natural frequencies in vibration may be underestimated (even though the mode shapes are similar) in a SOL 103 in the absence of follower stiffness. To the contrary, this observations are reversed in case of centrifugal loads. Centrifugal forces as a constant (static) load are applied by a Bulk Data RFORCE to any elements that have masses. The follower stiffness due to centrifugal load has the effect of lowering stiffness (although the centrifugal load tensioning effect increases stiffness), consequently lowering natural frequencies (even though the mode shapes are similar) in a SOL 103 and lowering the buckling loads (even though the mode shapes are similar) in a SOL 105. This effect increases as the RPM increases, and it becomes significant when the RPM is over 1000. For moderately geometric nonlinear analysis, exclusion of follower stiffness affects the rate of convergence, but the converged solution is correct. For severely geometric nonlinear analysis, it may not be possible to obtain a converged solution without including follower stiffness. As the geometric nonlinearity intensifies, so is the effect of follower stiffness. Therefore, inclusion of follower stiffness greatly enhances the convergence if the deformation involves severe geometric nonlinearity. 294 Structural Engineering Analysis and Design Second Edition 4.1.2.3 GL, ML P-∆ (KGA From Exact or Approximate KTA) Real Modal Analysis It is often necessary to include the differential stiffness, especially if there are prestressed cables in the model and the mode shapes are sought. Modal Dynamic P - ∆ [[ K TA ] − ω ni [M ]]{φ}i = {0} 2 To obtain KTA, to be theoretically exact, a GNL SOL 106 (or implicit dynamic relaxation SOL 129 or explicit dynamic relaxation LS-DYNA) with prestress (as temperature loads say) and gravity must be undertaken. Alternatively, an approximation to KTA can be obtained by repetitive P-∆ static analyses with the prestress (as temperature loads say) and gravity applied. The procedure to obtain this approximate KTA will be presented. Note that the approximate KTA will be the summation of the elastic stiffness KE at the undeflected (by the prestress and gravity) state but KG at the deflected (by the prestress and gravity) state. Hence if KE changes considerably during the application of the prestress, a full SOL 106 (or implicit dynamic relaxation SOL 129 or explicit dynamic relaxation LS-DYNA), which converges to the KE and KG at the deflected (by the prestress and gravity) state should be employed. Hence for the modelling of a suspension bridge where there is a great change in geometry (known in the bridge industry as form-finding, so-called because it is necessary to find the form or shape of the catenary suspension cables), it may be prudent to employ SOL 106 (or implicit dynamic relaxation SOL 129 or explicit dynamic relaxation LS-DYNA), but for a high tension low sag cable on say a tower with prestressed cables, the repetitive P-∆ static analysis may be adequate. The repetitive P-∆ analysis basically involves a number of iterations of linear static analyses to obtain an approximate KTA. Note again that A refers to the initial undeflected (by the collapsing load) state, but deflected by the prestress and gravity. To perform the repetitive P-∆ analysis, a static analysis is performed based on KEA with temperature loads and gravity to generate forces in the structural elements, which in turn provides input for the computation of KGiAKTm where m is the iterations. Repetitive static analysis is performed with the prestress and gravity updating the stiffness matrix KEA + KGiAKTm-1 + KGiAKTm until convergence of displacements is obtained. The tangent stiffness at this stage is the approximate converged tangent stiffness matrix KTA = KEA + KGiAKT. The converged displacements represent the approximate P∆ (KGA From Approximate KTA) static response to the initial prestress loads. The converged geometric stiffness at this stage would be that based upon the approximate tangent stiffness matrix KTA, i.e. KGiAKT. Phase 1 Perform static analysis (with prestress and gravity) based on [KEA] but include the segyroa.v2001 alter prior to the Case Control Section in order to compute the geometric stiffness matrix [KGA]1 (and output into a .pch file) based on the generated element loads from the [KEA] static analysis. Phase 2 Perform static analysis (with prestress and gravity) based on [KEA] + [KGA]1 by including the k2gg = ktjj statement in the Case Control Section, the outputted .pch file which contains the ktjj matrix in the Bulk Data and the segyroa.v2001 alter prior to the Case Control Section to compute the [KGA]2 (and output into the .pch file overwriting previous data) based on the generated element loads from the [KEA] + [KGA]1 static analysis. Phase 3 Repeatedly perform the Phase 2 static analysis (with prestress and gravity) based on [KEA] + [KGA]i for i = 2 to n where n represents the number of iterations required for the change in deflections between analyses to become negligible. This would signify that the change in the [KGA] matrix become negligible and the correct [KGA] is attained. The deflections and the other responses at this stage represent the P-∆ (KGA From Approximate KTA) static response to the prestress and gravity. The stiffness of the structure is KTA. Phase 4 A SOL 103 is undertaken with the k2gg=ktjj statement in the Case Control Section and the outputted .pch file which contains the latest ktjj matrix in the Bulk Data. The responses at this stage represent the P-∆ (KGA From Approximate KTA) real modal response. 295 Structural Engineering Analysis and Design Second Edition 4.1.3 4.1.3.1 Hand Methods Verification Natural Frequency and Free Vibration Response of SDOF Systems Equation of motion m& u&( t ) + ku ( t ) = 0 Assume general solution u(t) = Ge λt where G = G R + iG I and λ = α + iωd Hence mGλ2 e λt + kGe λt = 0 (mλ 2 ) + k Ge λ t = 0 for LHS to be zero for all t (mλ ) λ1 = +i k m + k = 0 as Ge λt > 0 the roots of this quadratic characteristic equation are 2 k m λ 2 = −i ∴α = 0 and ωd = ω n = k rad / s m note that the relationships, natural frequency, f n = 2π ωn Hertz and the period, Tn = s 2π ωn hence, the complementary function, u(t) = G1e λ1t + G 2 e λ 2 t u(t) = (G1R + iG1I )(cos ωn t + i sin ωn t ) + (G 2 R + iG 2I )(cos ωn t − i sin ωn t ) u ( t ) = [((G1R + G 2 R )cos ωn t − (G1I − G 2 I )sin ωn t ) + i((G1I + G 2 I ) cos ωn t + (G1R − G 2 R )sin ωn t )] the free vibration response must be real for all t, hence G1I = −G 2 I and G1R = G 2 R sin ce there are two less independent constants, let G1I = −G 2 I = G I and G1R = G 2 R = G R we notice that G1 and G 2 are a complex conjugate pair G1 = G R + iG I and G 2 = G R − iG I hence the general solution u ( t ) = 2G R cos ωn t − 2G I sin ωn t Substituti ng the integration constants with the initial conditions, u&(0) u ( t ) = u (0) cos ωn t + sin ωn t ωn Hence the maximum dynamic displacement 2 u max  u&(0)   + u (0) 2 =  ω  n  296 Structural Engineering Analysis and Design Second Edition A free vibrational dynamic response analysis involves initial displacement and velocity conditions but no forcing vector. It is important to realize that the vibration occurs about the static equilibrium position. Hence we always define u(t) to begin from the static equilibrium position. However, the dynamic analysis need not begin at this point. For example, in the instance of a mass m on a string of tensile stiffness k dropped from a level where the string is not taut, the dynamic analysis begins (t = 0.0) when the string just becomes taut and hence u(t = 0.0) = −mg/k and du/dt (t = 0.0) will be the velocity of the mass when it reaches that particular taut string elevation. Likewise, when a mass m is dropped h meters onto the tip of a cantilever, u(t = 0.0) = −mgL3/(3EI) and du/dt (t = 0.0) = (2gh)1/2. The static displacement was found simply from the force mg divided by the stiffness 3EI/L3. From the knowledge of the initial conditions, we can determine the maximum dynamic displacement by solving the free vibrational dynamic equation of motion. In summary, to determine the maximum dynamic displacement, (i) first identify the u(t) = 0 reference as the position of static equilibrium; (ii) second, identify the t = 0 level as when dynamic analysis begins, i.e. when a dynamic equation of motion can be written down (iii) evaluate the initial conditions u(t = 0.0) and du/dt (t = 0.0) (iv) evaluate the natural circular frequency of the system (iv) the maximum dynamic displacement can be ascertained from the formula To estimate the undamped natural circular frequency, we employ ωn=(k/m)0.5. The single mass m is readily obtainable for SDOF systems. The elastic stiffness in the direction of the dynamic freedom k is obtained from either of the following methods. 4.1.3.1.1 Natural Frequency Using the Unit Load Method (Virtual Work) P ∆ = f δ expresses virtual work i.e. external work = internal work P’∆ = f ’δ expresses the load method where P’ = virtual external action, specified usually as unity for the unit load method ∆ = real external kinematic, the item to be found f ’ = virtual internal action, due to the virtual external actions P’ δ = real internal kinematic, due to the real external actions on the structure 1’∆ = f1’δ expresses the unit load method 1’∆1 = f1’δ1 represents the unit load method with the real external actions also unity i.e. both the virtual external actions and real external actions are unity ∆ 1 = external real kinematic due to unit external real action = f1 ' δ 1  T  M   P  P L V Q  = ∫ (M 1 )V  1 ds  + ∫ (P1 )V  1 ds  or (P1 )V  1  + ∫ (T1 )V  1 ds  + ∫ (V1 )V  1 ds  EI EA EA GK  R  R  R  GIb  R t  R + (P 1spring = ∫ M1 k=  P1spring  V  k spring )   M  + (M 1spring )  1spring V  rotational  k spring R      T1spring ( )  + T1spring V  torsional   k spring R      R P1sp M 1sp T1sp M1 P PL T VQ ds + ∫ P1 1 ds or P1 1 + ∫ T1 1 ds + ∫ V1 1 ds + P1sp + M 1sp + T1sp EI EA EA GK t GIb k sp k rot sp k tor sp 1 ∆1 To estimate the undamped natural circular frequency, we employ ωn=(k/m)0.5. If αs > 0 and given BMD for non-unity external action, say for a load of 700. 1’∆ = f1’δ expresses the unit load method. δ700 is given, and to find f1, simply randomly release any indeterminacy to draw the virtual internal action 297 Structural Engineering Analysis and Design Second Edition diagram f1 removing the real external load 700 and applying the virtual external unit load. Then, ∆700 = f1’δ700 and finally, k = 700 / ∆700. To estimate the undamped natural circular frequency, we employ ωn=(k/m)0.5. 4.1.3.1.2 Natural Frequency Using Stiffness Formulae It is worth noting that the equivalent stiffness of springs in parallel is the addition of the individual stiffnesses and the equivalent stiffness of springs in series is the inverse of the addition of the inverse of the individual stiffnesses. Stiffness in series occurs when the load path has to travel both stiffnesses sequentially. Stiffness in parallel occurs when the load path is given the option to be more attracted to the stiffer element. In series, there is no question of whether the load will travel the path or not, for it must, all loads must travel some path, and in series, there is no other option. A mass on the bottom of a vertically hanging spring at the free end of a bending beam cantilever can be idealized as a SDOF system with equivalent springs in series. 1 1 L3 = + k e k spring 3EI Single story shear frames can be idealized as SDOF systems with the stiffness from the bending beam columns equivalent to a system of springs in parallel because of the axial rigidity of the horizontal member of the shear frame. By definition, there is full moment rigidity between the top of the columns and the rigid horizontal member. Standard fixed ended bending beam lateral stiffness used for shear frames with fixed bases is k = number of columns x 12EI/L3. Standard cantilever bending beam lateral stiffness used for shear frames with pinned bases, k = number of columns x 3EI/L3. An example of a shear frame includes water tank towers. To estimate the undamped natural circular frequency, we employ ωn=(k/m)0.5. 4.1.3.1.3 Natural Frequency Using the Static Deflection (used when EI not readily available) The natural frequency can be estimated from 1 k 2π m Replacing the mass term with weight, W, we have fn = fn = g 2π g k = mg 2π g k 1 = = 15.76 W 2π u st u st u st in mm Which now relates the natural frequency to the static deflection ust of a single lumped mass dynamic DOF. This formula is exact for single lumped mass systems. 298 Structural Engineering Analysis and Design Second Edition 4.1.3.2 Natural Frequencies of MDOF Systems Either the stiffness or flexibility formulation to the equation of motion can be employed. The solution can be performed by either the exact classical determinant method, the approximate Stodola iterative method, the approximate Rayleigh Quotient method or the approximate Rayleigh-Ritz method. 4.1.3.2.1 Stiffness Formulation Shear frames analysis assumes that the mass of the structure is concentrated at the floors, that the axial force in the columns are too small to consider axial deformation, and that the floor girders are infinitely stiff compared to the columns such that there is no rotation at the connection between the floor and the columns. The third assumption means that the stiffness (or flexibility) of the structure is only provided by the columns. The free, undamped vibration of the shear frame is described by the equation of motion [M] {ü(t)} + [K] {u(t)} = {0} The [K] matrix can be the instantaneous stiffness matrix [KEA] or the tangent stiffness matrix [KTA], the A denoting at its initial undeflected configuration. In the instantaneous stiffness matrix, the stiffness coefficient kij is the force required at the ith coordinate to maintain a unit displacement at the jth coordinate while all other coordinates remain stationary. Formulate [KEA] column-by-column (each column corresponding to a unit displacement at the jth coordinate) noting the forces required in all the i coordinates. Ensure [KEA] is symmetric. M1 h1 h2 u1 EI1 M2 M1 [M ] =  0  0 u2 EI2 M3 u3 h3 0 M2 0 0  0  M 3  EI3 A unit displacement of u1 would induce a force of 2x12EI1/h13 at DOF 1 and a force of -2x12EI1/h13 at DOF 2 for all other DOFs to remain stationary. A unit displacement of u2 would induce a force of 2x12EI1/h13+2x12EI2/h23 at DOF 2, a force of -2x12EI1/h13 at DOF 1 and a force of -2x12EI2/h23 at DOF 3 for all other DOFs to remain stationary. A unit displacement of u3 would induce a force of 2x12EI3/h33 at DOF 3 and a force of -2x12EI2/h23 at DOF 2 for all other DOFs to remain stationary. Hence, the instantaneous stiffness matrix,  24EI1  3  h1  24EI1 [K AE ] =  − h 13   0   − 24EI1 h 13 24EI1 h 13 − + 24EI 2 h 32 24EI 2 h 32    24EI 2  −  3 h2  24EI 2 24EI 3  + h 32 h 33  0 Note that the stiffness contributions from the columns at the same level are added because the stiffnesses are in parallel to each other. Also, had a base been pinned, then the lateral stiffness contribution would just be 3EI/h3 instead of 12EI/h3. 299 Structural Engineering Analysis and Design Second Edition It may also be prudent to include the reduction in stiffness from the P-∆ effect, i.e. a linearized geometric stiffness matrix. A unit displacement of u1 would induce a secondary moment of M1g in the topmost columns (note all the topmost columns and not just one of them) for all other DOFs to remain stationary. This can be represented by a force M1g/h1 at DOF 1 and a force -M1g/h1 at DOF 2. Likewise, a unit displacement of u2 would induce a secondary moment of M1g in the topmost columns and a secondary moment of (M1+M2)g in the intermediate columns. This can be represented by a force -M1g/h1 at DOF 1, a force M1g/h1+(M1+M2)g/h2 at DOF 2 and a force -(M1+M2)g/h2 at DOF 3. Finally, a unit displacement of u3 would induce a secondary moment of (M1+M2)g in the intermediate columns and a secondary moment of (M1+M2+M3)g in the lowermost columns. This can be represented by a force (M1+M2)g/h2 at DOF 2 and a force (M1+M2)g/h2+(M1+M2+M3)g/h3 at DOF 3. Hence, the geometric stiffness matrix,  M 1g   h1 Mg A [K Gn ] =  − 1 h1   0  M 1g h1 M1g (M1 + M 2 )g + h1 h2 ( M1 + M 2 )g − h2 −    ( M1 + M 2 )g  −  h2 (M1 + M 2 )g + (M1 + M 2 + M 3 )g   h2 h3 0 It is important to point out that the instantaneous stiffness matrix represents the forces required to produce and maintain the unit displacements in the pertinent DOFs. The geometric stiffness matrix on the other hand represents the forces which are generated due to the unit displacements in the pertinent DOFs. Hence the equation of motion is [M] {ü(t)} + [KEA] {u(t)} = [KGnA] {u} [M] {ü(t)} + [[KEA]−[KGnA]] {u(t)} = {0} [M] {ü(t)} + [KT] {u(t)} = {0} Letting {u}i = {φ}i Gieλit leads to the real eigenvalue problem [[K] − ωni2 [M]]{φ}i = 0 The total solution of the free vibrational problem is given by the linear superposition of the individual modes of vibration.  A1 sin(ω1 t − α1 )    Μ   {u} = [{φ}1... {φ}i ... {φ}n ] A i sin(ωi t − α i )    Μ   A n sin(ω n t − α n )  The constants Ai and αi are the constants of integration to be determined from the initial displacement and velocity conditions. Note that the flexibility matrix [F] of the frame can be obtained from a linear static analysis program by successively applying unit loads at each storey and on each occasion measuring the total displacement at all the storey levels. The matrix [F] is then inversed to obtain the stiffness matrix [K]. 300 Structural Engineering Analysis and Design Second Edition 4.1.3.2.2 Flexibility Formulation Stiffness formulation, [[K ] − ω 2ni [ M ]]{φ}i = {0} Multiply by [F] or by − 1 [ F], ω 2ni [[F][K ] − ω 2ni [ F][M ]]{φ}i = {0} or [[F][ M ] − 1 [ F][K ]]{φ}i = {0} ω 2ni [[I] − ω 2ni [ F][M ]]{φ}i = {0} [[F][ M ] − 1 [ I]]{φ}i = {0} ω 2ni or ( Flexibility formulations) These are eigenvalue problems. Flexibility coefficient fij is the displacement produced at the ith coordinate due to a unit force applied at the jth coordinate only. Formulate [F] column-by-column (each column corresponding to a unit force at the jth coordinate) noting the displacements induced in all the i coordinates. In formulating these columns in [F], 3 cases are identified: (a) Unit force above the displacement of the DOF sought Displacement of the DOF is the flexibility of all that including and below the displacement DOF (b) Unit force inline with the displacement of the DOF sought Displacement of the DOF is the flexibility of all that including and below the displacement DOF (c) Unit force below the displacement of the DOF sought Displacement of the DOF is the flexibility of all that including and below the unit force In short, the displacement at the particular DOF sought after is the cumulative flexibility (inverse of stiffness) of all the shear frame levels including and below the displacement DOF or the unit force, whichever is lower. Ensure F is symmetric. M 3m 3m 3m M M u1 u1 12EI/3 EI 3 3 12EI/3 u2 u2 EI 12EI/33 12EI/33 u3 12(2EI)/33 12(2EI)/33 u3 2EI Transverse stiffness of columns 9 9  9  8EI + 8EI + 16EI  9 9 [F] =  +  8EI 16EI 9   16EI 9 9 + 8EI 16EI 9 9 + 8EI 16EI 9 16EI 9  16EI  5 3 1 9  9  = 3 3 1 16EI  16EI  1 1 1 9   16EI  301 1 9 = 3 8EI 12EI / 3 + 12EI / 3 3 1 9 = 3 8EI 12EI / 3 + 12EI / 3 3 1 9 = 12(2EI) / 3 3 + 12(2EI) / 3 3 16EI Displacement contribution of floor level due to unit load at the particular level M 0 0  [M ] =  0 M 0   0 0 M  Structural Engineering Analysis and Design Second Edition 4.1.3.2.3 Natural Frequencies Using the Exact Classical Determinant Method The stiffness formulated real eigenvalue problem is expressed [[K] − ωni2 [M]]{φ}i = 0 This equation has one additional unknown and hence does not have a unique solution. For a 3 DOF dynamic system, there will be 3 φ terms and the ωni2 term, i.e. one additional unknown. For there to be a solution that is nontrivial (i.e. that not all φ terms zero), the determinant must be zero. The eigenvalue problem is solved for ωni2 by employing the classical determinant computation for a nontrivial solution, Det [[K] − ωni2 [M]] = 0 This leads to a polynomial in ωni2 the order of which corresponds to the number of dynamic degrees of freedom. For instance, for a 3 DOF dynamic system, the order of polynomial in ωni2 will be cubic, i.e. up to the ωni6 term. They can be solved for the 3 natural circular frequencies ω1, ω2 and ω3. Then, in order to obtain the an eigenvector corresponding to each eigenvalue, we replace each eigenvalue in turn into [[K] − ωni2 [M]]{φ}i = 0 Now that we have found ωni2 based on a zero determinant, the number of independent equations becomes one less, i.e. for the 3 DOF dynamic system, 2 independent equations. Hence for each ωni2 we can solve for the relative values of φ. This is where we have to decide on how to normalize the eigenvectors, i.e. whether MAX, MASS or POINT normalization. Note that the first mode or fundamental mode refers to the mode corresponding to the lowest frequency. The other modes are referred to as higher harmonics. The flexibility formulated real eigenvalue problem is expressed [[I] − ω 2ni [ F][M ]]{φ}i = {0} or [[F][ M ] − 1 [ I]]{φ}i = {0} ω 2ni These are eigenvalue problems. For a nontrivial solution, DET[[ I] − ω2ni [ F][M ]] = 0 or DET[[F][M ] − 302 1 [ I]] = 0 ω 2ni Structural Engineering Analysis and Design Second Edition 4.1.3.2.4 Natural Frequencies Using the Approximate Stodola Iterative Method With this method, only the fundamental natural circular frequency and the fundamental mode can be obtained fairly accurately. Higher natural circular frequencies and modes can also be obtained inefficiently with the use of the sweeping matrix to purify the eigenvalue problem off the earlier modes of vibration. However, this method is subjected to cumulative errors and so the errors increase in estimating the frequencies and mode shapes of higher modes of vibration. Stiffness formulation, [K − ω 2 M ]φ = 0 Multiply by F or by − 1 F, ω2 [FK − ω 2 FM ]φ = 0 or [FM − 1 FK ]φ = 0 ω2 [I − ω 2 FM ]φ = 0 or [FM − 1 I]φ = 0 ω2 ( Flexibility formulations) Employ the latter flexibility formulation, [FM − 1 I]φ = 0 ω2 FM φ = 1 φ ω2 Stodola ' s method, FM φ = 1 φ is akin to A x = λ x ω2 Guess x (0 ) For i = 0 to n Compute A x (i ) Normalise first coordinate of A x (i ) to obtain λ(i +1) and x Next i The final λ(n +1) is the 1 ( n +1) and x the fundamental mode φ1 . ω12 303 ( i +1) Structural Engineering Analysis and Design Second Edition M 3m u1 EI M 3m 12EI/33 1 9 = 3 12EI / 3 x 2 8EI 3 3 12EI/3 1 9 = 3 12EI / 3 x 2 8EI 12(2EI)/33 12(2EI)/33 1 9 = 3 12(2EI) / 3 x 2 16EI 3(4EI)/43 3(4EI)/43 1 8 = 3 3(4EI) / 4 x 2 3EI u2 EI 1.5M 3m 12EI/33 12EI/3 u3 2EI 2M u4 4EI 4m Displacement contribution of floor level due to unit load at the particular level Transverse stiffness of columns The figure above shows a 4-degree of freedom shear frame. The flexibility formulation is described by 1 [FM − 2 I]φ = 0 ω FM φ = 1 φ ω2 Stodola ' s method, 1 FMφ = 2 φ is akin to A x = λ x ω (0) Guess x For i = 0 to n Compute A x (i ) Normalise first coordinate of A x (i ) to obtain λ(i +1) and x ( i +1) Next i The final λ(n +1) is the 1 ( n +1) and x the fundamental mode φ1 . ω12 For the shear frame above, 9 9 8  9  8EI + 8EI + 16EI + 3EI  9 9 8  + + F =  8EI 16EI 3EI 9 8  +  16EI 3EI  8  3EI  M 0 0 M M= 0 0   0 0 9 9 8 + + 8EI 16EI 3EI 9 9 8 + + 8EI 16EI 3EI 9 8 + 16EI 3EI 8 3EI 9 8 + 16EI 3EI 9 8 + 16EI 3EI 9 8 + 16EI 3EI 8 3EI 0  0  3 M 0  2  0 2M  0 0 304 8  3EI   263 8    3EI  = 1  209 8  48EI 155  3EI  128 8   3EI  209 155 128 209 155 128 155 155 128  128 128 128 Structural Engineering Analysis and Design Second Edition Hence,  263  1  209 A = FM = 48EI 155  128  263  M  209 = 48EI 155  128  1  0.8000 , Guess x ( 0) =  0.7000   0.6000  1  0.9277  , x (1) =  0.7975   0.6944  1  0.9342 ( 2) , x = 0.8072   0.7044  1  0.9346 ( 3) , x = 0.8082   0.7055 209 155 128 M 0  209 155 128  0 M 155 155 128  0 0  128 128 128  0 0 0  0 0  3 M 0  2  0 2M  0 209 232.5 256 209 232.5 256 155 232.5 256  128 192 256  263  M 209 A x (0) = 48EI 155  128  263  M 209 A x (1) = 48EI 155  128  263  M  209 ( 2) Ax = 48EI 155  128  263  M 209 ( 3) Ax = 48EI 155  128 209 232.5 256  1   1  15.5531      209 232.5 256 0.8000 M 14.4281 15.5531M 0.9277  = = 0.7975 155 232.5 256 0.7000 EI 12.4031 EI       128 192 256 0.6000 0.6944 10.8000 209 232.5 256  1   1  17.0846      209 232.5 256 0.9277  M 15.9596 17.0846M 0.9342 = = 0.8072 155 232.5 256  0.7975 EI 13.7909 EI       128 192 256 0.6944 0.7044 12.0338 209 232.5 256  1  17.2132  1       209 232.5 256 0.9342 M 16.0882 17.2132M 0.9346 = = 0.8082 155 232.5 256 0.8072 EI 13.9123 EI       128 192 256 0.7044 12.1432 0.7055 209 232.5 256  1  17.2261  1       209 232.5 256 0.9346 M 16.1011 17.2261M 0.9347  = =  0.8083 155 232.5 256 0.8082 EI 13.9246 EI       128 192 256 0.7055 12.1544 0.7056  Convergence is achieved to two decimal places. Thus, 1 17.2261M = , EI ω12 EI EI = 0.2409 17.2261M M  1  0.93 . and the fundamental mode φ1 =  0.81   0.71 fundamental frequency ω1 = For higher modes the sweeping matrix can be employed. This method is computationally intensive and the rate of convergence depends very much on whether the initial guessed mode shape approximates the actual mode shape sought after. Also the errors are cumulative as the sweeping matrix is a function of the previous mode shape. Hence, higher modes are less accurate. As will be demonstrated hereafter, the first and second modes converge to the exact solution to 3 decimal places, whilst the third mode shape is only accurate to 2 decimal places. 305 Structural Engineering Analysis and Design Second Edition M 3m u1 u1 EI M 12EI/33 12EI/33 u2 12EI/33 12EI/33 u3 12(2EI)/33 12(2EI)/33 u2 3m EI M u3 3m 2EI Transverse stiffness of columns 1 9 = 12EI / 3 3 + 12EI / 3 3 8EI 1 9 = 12EI / 3 3 + 12EI / 3 3 8EI 1 9 = 3 12(2EI) / 3 + 12(2EI) / 3 16EI 3 Displacement contribution of floor level due to unit load at the particular level The figure above shows a 3-degree of freedom shear frame. The flexibility formulation is described by FMφ = 1 φ ω2 5 3 1  M 0 0  9  A = FM = 3 3 1  0 M 0  16EI  1 1 1  0 0 M  Ax = λx Fundamental mode : Operate on A = FM Guess x (0) 1  = 0.7 ,  0.3 Ax ( 3) 1.0000  4.1984M   = 0.7320 EI 0.2680 Convergence is achieved to 4 decimal places after 3 iterations. Thus, 1/ω12 = 4.1984M / EI, EI EI T and the fundamental mode φ1 = [1 0.7320 0.2680]. = 0.4880 M 4.1984M fundamental frequency ω1 = Sweeping matrix, S1 = I − 1 φ1 φ1T M where Μ 1 = φ1T M φ1 Μ1 Second mode : Operate on A = FMS1 Guess x (0)  1  = − 0.8, − 0.8 Ax (12)  1.0000  0.5625M   = − 0.9994 EI  − 0.9995 Convergence is achieved to 4 decimal places after 12 iterations. Thus, 1/ω 22 = 0.5625M / EI, EI EI T and the second mode φ 2 = [1 − 0.9994 − 0.9995] = 1.3333 0.5625M M 1 T T Sweeping matrix, S 2 = S1 − φ 2 φ 2 M where Μ 2 = φ 2 M φ 2 Μ2 ω2 = Third mode : Operate on A = FMS 2 Guess x (0) 1  = − 2,  3  Ax ( 3)  0.9999  0.3014M   = − 2.7358 EI  3.7360  Convergence is achieved to 4 decimal places after 3 iterations. Thus, 1/ω 32 = 0.3014M / EI, ω3 = EI EI T and the third mode φ 3 = [0.9999 − 2.7358 3.7360] = 1.8215 0.3014M M 306 Structural Engineering Analysis and Design Second Edition 4.1.3.2.5 Natural (Fundamental) Frequency Using the Approximate Rayleigh Quotient Method The stiffness formulated eigenvalue problem can be solved by employing the Rayleigh Quotient method. The basis of the method is to equate the maximum kinetic energy during motion to the maximum potential energy to obtain an estimate of the natural circular frequency with an assumed mode shape or displacement function. With this method, only the fundamental natural circular frequency can be obtained fairly accurately. Vibration analysis by Rayleigh’s Quotient method will yield a fundamental natural circular frequency ω1 which is higher than the actual because of the approximation made by the mode shape φ(x). Higher natural circular frequencies can be obtained only if the exact higher mode shapes are known. Improved Rayleigh Quotient Method (a) Guess mode shape based on the displacements produced by applying inertial forces as static loads. That is to say, load the structure with the inertial loads associated with an assumed displacement. This load then results in a new improved displacement configuration. Loop for even better estimate or simply goto (b). (b) Apply Rayleigh’s formula to obtain an estimate of ωi {φ } [K ]{φi } = Generalised Stiffness of Mode i, K i = iT Generalised Mass of Mode i, Mi {φi } [M ]{φi } T ωi2 = ∑ k ∆φ ∑m φ i 2 i 2 i i (c) From the obtained estimate of the eigenvalue, obtain a better estimate of the eigenvector from [[K] − ωni2 [M]]{φ}i = 0 with the eigenvector normalized in the same method as before. Loop to (b) for a new estimate of the eigenvalue based on the new eigenvector. This is repeated until convergence. The stiffness of the calculated system is always greater than the stiffness of the exact system as we are modelling a system of infinite DOFs with a finite number of DOFs. The value of ω1 decreases as the mode shape becomes closer to the actual fundamental mode shape. Hence, the calculated natural circular frequency will always be greater than the exact value. Seek to obtain the lowest possible estimate of ω for convergence. M 3m M 3m u1 EI u2 0.8 EI 1.5M 3m 1.0 2M u3 0.7 2EI u4 0.6 4EI 4m Assumed Mode Shape Freedom Assumed Mode Shape Force on the Freedoms Miφiω2 Force on Shear Frame (Cumulative) Displacement Contribution of Floor Level Displacement of Shear Frame (Cumulative) Improved Mode Shape 1 2 3 4 1.0 0.8 0.7 0.6 Mω2 0.8Mω2 1.5M(0.7ω2) 2M(0.6ω2) Mω2 1.8Mω2 2.85Mω2 4.05Mω2 Mω2/(24EI/27) 1.8Mω2/(24EI/27) 2.85Mω2/(48EI/27) 4.05Mω2/(24EI/64) 15.55Mω2/EI 14.43Mω2/EI 12.40Mω2/EI 10.80Mω2/EI 1 0.93 0.80 0.69 307 Structural Engineering Analysis and Design Second Edition 12 EI   2 × 33   − 2 × 12 EI 33 K=  0    0  M 0 M= 0  0 12 EI 33 12 EI 4× 3 3 12 EI − 2× 3 3 − 2× 0 0 0 M 0 0 1 .5 M 0 0 0  0  0   2M  0 12 EI 33 12( 2EI) 12 EI 2× 3 + 2× 3 33 12( 2EI) − 2× 33  1  0.93   φ1 =   0.80  0.69  − 2×   24   27   24  0 −  = EI  27  12( 2EI)  − 2×  3  0 3   12( 2 EI) 3(4 EI)   0 2× + 2 ×  33 4 3  0 24 27 48 27 24 − 27 − 0 0 24 27 8 3 48 − 27 −  0   0   48  −  27 155   72  Hence, the fundamental natural circular frequency ω1 is given by ω12 = K1 {φ }T [K ]{φ1 } = 0.2194EI = 0.0581 EI = 1T M1 {φ1 } [M ]{φ1 } 3.7771M M ∴ ω1 = 0.2410 EI M The alternative approach to the calculation is to use the following formula. However, the former approach above is more recommended as defining the storey stiffnesses below can be tricky. ω12 = ∑ k ∆φ ∑m φ i i 2 i 2 i 12EI/33 12EI/33 12EI/33 12EI/33 12(2EI)/33 12(2EI)/33 3(4EI)/43 3(4EI)/43 Transverse stiffness of columns ω12 = ∑ ∑m φ k i ∆φ i2 i = 2 i  12(2EI)   3(4EI)   12EI   12EI  2 2 2 2 (0.80 − 0.69) +  2 x (0.69)  2 x 3 (1.0 − 0.93) +  2 x 3 (0.93 − 0.80) +  2 x 3 3  3  3 43       = M x 1.0 2 + M x 0.93 2 + 1.5M x 0.80 2 + 2M x 0.69 2 0.2194EI EI = 0.05809 3.7771M M ω1 = 0.05809 EI EI = 0.2410 M M 308 Structural Engineering Analysis and Design Second Edition Rayleigh Quotient Method – No Improvement To Guessed Mode Shape The Rayleigh Quotient expression can also be rewritten in terms of the static displacements as follows. This is employed in Earthquake Engineering codes of practice for the fundamental period of structures. T1 = 2π ∑Wδ g∑ W δ 2 i i i i The static deflections due to the horizontal application of the weight of the structure are obtained from a static analysis program. It need not be the gravity forces that are applied, but any inertial force that produces a deflected shape corresponding to the mode shape of interest. The static horizontal deflected shape of the structure resembles the fundamental mode shape of the vibrational analysis because the p0i/Ki term is largest for the fundamental mode since higher modes are less significant in contributing to the static response. This method however does not employ the repetitive improved estimates of the Improved Rayleigh Quotient method until convergence of the mode shape. Hence if the mode shape estimate is incorrect, so will be the natural frequency. Of course, the static displacement should be calculated assuming a weight corresponding to the loading for which the frequency is required, i.e. usually a dead load with an allowance for the expected live load. Vertical bending modes of single span beams and plates can be found knowing the static deflections at various points (hence assuming lumped mass DOFs at those points). For the horizontal mode of vibration of an entire structure, the gravity force must be applied laterally. For multi-span beams, say a two span continuous beam, the fundamental mode is an antisymmetric mode. Hence, if the static loads were applied all in the same direction, we would be predicting the frequency of the symmetric mode, which is higher. This is an example where the assumed mode shape was totally incorrect. The repetitive improved estimates of the Improved Rayleigh Quotient method above would have detected this. The static load should have been applied downwards in one span and upwards in the other to produce a deflected shape that somewhat resembles the fundamental asymmetric mode. Lumped Mass Rayleigh Quotient Method – Lumped Mass & No Improvement To Guessed Mode Shape The above Rayleigh Quotient expression can also be rewritten in terms of the static displacement and lumping the mass to a single mass DOF. For SDOF systems, we have said that the natural frequency can be estimated from 1 k 2π m This is the Rayleigh Quotient expression for SDOF systems if you like. Replacing the mass term with weight, W, we have fn = fn = g 2π g k = mg 2π g k 1 = = 15.76 W 2π u st u st u st in mm Which now relates the natural frequency to the static deflection ust of a single lumped mass dynamic DOF. This formula is exact ONLY for single lumped mass systems. We can approximately extend this to MDOF systems but the numerical factor 15.76 will be different generally between 16 and 20; 18 is quite practical. But of course, this is a fudge to account for the fact that we are not taking static deflections at various mass DOFs, but simply at one solitary mass DOF. The advantage of this method is that it is simple. If the static deflection is known from various standard static deflection equations, the natural frequency can be determined, albeit very approximately. Vertical bending modes of single span beams and plates can easily be found knowing the midpoint static deflection (hence assuming a lumped mass DOF in the middle). For the horizontal mode of vibration of an entire structure, the gravity force must be applied laterally and the lateral deflection at the top of the equivalent vertical cantilever is employed (hence assuming that the lumped mass DOF is at the top of the building). 309 Structural Engineering Analysis and Design Second Edition 4.1.3.2.6 Natural Frequencies Using the Rayleigh-Ritz Method The Rayleigh Quotient method gives the first mode of vibration only. Ritz extended this method to give a few more modes. The full eigenvalue problem is expressed as ([K] − ωi2[M]) {φi} = {0} i = 1 to the number of DOF in original system, n But with the approximation of {φ} = [Ψ]{z}, the reduced eigenvalue problem can be expressed as ([K*] − ωi2[M*]) {zi} = {0} i = 1 to the number of Ritz vectors in reduced system, s < n Hence, the following procedure is undertaken (a) [K] and [M] are established (b) The Ritz vectors [Ψ] = [{Ψ1},{Ψ2},…{Ψs}] are assembled, where s < n (c) Compute [K*] = [Ψ]T[K][Ψ] and [M*] = [Ψ]T[M][Ψ] (d) Solve the reduced eigenvalue problem ([K*] − ωi2[M*]) {zi} = {0} Det ([K*] − ωi2[M*]) = 0 Hence, ωi and {zi} obtained, i = 1 to s (e) The s (not n) approximate mode shapes in the original system is obtained {φi} = [Ψ]{zi} obtained, i = 1 to s (f) The number of good approximation of modes = s / 2; Hence, Ritz extended Rayleigh’s method to give s / 2 modes with good accuracy 310 Structural Engineering Analysis and Design Second Edition 4.1.3.3 Natural Frequencies of Distributed Systems 4.1.3.3.1 Natural (Fundamental) Frequency Using the Approximate Rayleigh Quotient Method The Rayleigh Quotient Method is approximate because of the approximation of the mode shape. The closer the mode shape resembles the true mode shape, the more accurate the natural frequency estimation. For the flexural Bernoulli-Euler beam of length L with additional lumped masses and stiffnesses the natural circular frequency ωi is given by ωi2 = Generalised Stiffness K i = Generalised Mass Mi ∫ L 0 ∫ L 0 n2 EI( x ){φ′′( x )} dx + ∑ k jφ2j 2 j=1 n1 m( x ){φ( x )} dx + ∑ m i φi2 2 i =1 The number of coefficients in the polynomial approximation of the mode shape φ(x) = the number of geometric and static boundary conditions + 1 One is added because one coefficient will cancel out in Rayleigh’s formula. Geometric boundary conditions: Fixed end Pinned end Free end in rotation and translation Free end with spring ks Free end in translation only φ(x) = 0 and φ′(x) = 0 φ(x) = 0 None None φ′(x) = 0 Static boundary conditions: Note that M(x) = EI(x)φ″(x) and V(x) = M′(x) = EI(x)φ″′(x) Fixed end None Pinned end φ″(x) = 0 Free end in rotation and translation φ″(x) = 0 and φ″′(x) = 0 φ″(x) = 0 Free end with spring ks Free end in translation only None 311 Structural Engineering Analysis and Design Second Edition 4.1.3.4 Natural Frequencies By Exactly Solving the Partial Differential Equilibrium Equation In reality, all systems have distributed mass, damping and stiffness properties. The finite element method discretizes the continuous system with a finite number of degrees of freedom resulting in a set of second order ordinary differential equations (ODEs). Continuous systems on the other hand result in one partial differential equation of at least second order. The reason for this is that on top of having the time variable, continuous systems also include the spatial variable as there are not discrete DOFs. Because of the mathematical complexity of generating and solving (integrating) these partial differential equations, this method is limited to simple structures. 4.1.3.4.1 The Bernoulli-Euler Beam The Bernoulli-Euler beam equation of motion, which is based on simple bending theory assuming that plane sections remain plane, no shear deformation and no axial force effects results in the equation of motion EI ∂4u ∂2u + m = P(x, t ) ∂x 4 ∂t 2 m = mass per unit length where u is the transverse displacement. Note that the Timoshenko beam equation extends the Bernoulli-Euler beam theory to include shear deformations and rotary inertia and should be used if such effects matter. Solving the corresponding free vibration PDE analytically by the method of separation of variables leads to two ODEs, which yield the following natural circular frequencies and mode shapes EI mL4 φ( x ) = A sin ax + B cos ax + C sinh ax + D cosh ax ω n = (aL ) 2 By applying various boundary conditions to these equations, various solutions may be found. The modal mass is Mi = m ∫ L 0 φ( x ) 2 dx Note that i refers to the natural modes, i = 1, 2, 3 … etc. Boundary Conditions (aiL)2 Term Natural Frequencies Fixed-Free (Cantilever) cos(aL)cosh(aL) – 1 = 0 thus (aiL)2 = 3.5160, 22.0345, 61.6972 … ωni = (a i L )2 EI mL4 Simply Supported sin(aL) = 0 thus, (aiL)2 = (iπ)2, i = 1, 2, 3 … ωni = (a i L ) EI mL4 Fixed-Simply Support (Propped Cantilever) tan(aL) – tanh(aL) = 0 thus (aiL)2 = 15.4118, 49.9648, 104.2477 … ωni = (a i L ) EI mL4 Free-Free cos(aL)cosh(aL) – 1 = 0 thus (aiL)2 = 22.3733, 61.6728, 120.9034 … ωni = (a i L ) EI mL4 Fixed-Fixed (Encastre) cos(aL)cosh(aL) – 1 = 0 thus (aiL)2 = 22.3733, 61.6728, 120.9034 … ωni = (a i L ) EI mL4 2 2 2 2 Mode Shapes Modal Mass φ i ( x ) = cosh a i x − cos a i x − σ i (sinh a i x − sin a i x ) σi = cosh a i L + cos a i L sinh a i L + sin a i L φi ( x ) = sin aix iπx = sin L L 0.25mL 0.50mL φi ( x ) = − cosh a i x + cos a i x + σi (sinh a i x − sin a i x ) M1 = 0.439mL − cosh a i L + cos a i L σi = − sinh a i L + sin a i L M 2 = 0.437 mL φ i ( x ) = cosh a i x + cos a i x − σ i (sinh a i x + sin a i x ) σi = M3 = 0.437 mL cosh a i L − cos a i L sinh a i L − sin a i L φ i ( x ) = cosh a i x − cos a i x − σ i (sinh a i x − sin a i x ) M1 = 0.394mL − cosh a i L + cos a i L σi = − sinh a i L + sin a i L M 2 = 0.439mL M 3 = 0.437 mL The modal mass for the simply supported beam is half the total mass for all the modes and that for the cantilever is quarter the total mass for all modes. 312 Structural Engineering Analysis and Design Second Edition The natural frequencies of a simply-supported Bernoulli-Euler beam with axial force (positive P being tension) are f ni = (iπ)2 2π EI mL4  PL2 1 +  EIi 2 π 2      313 Structural Engineering Analysis and Design Second Edition 4.1.3.4.2 The Shear Beam In reality, both shear and bending deformations must be accounted for when computing the frequencies of the beam. Shear deformation become prominent in deep (with respect to the span) beams. Hence the equivalent building cantilever beam model tends to be more of a shear mode. We are talking about the global behaviour of the building and not the shear deformation of individual column members, which are generally flexural. Note that shear frequencies are proportional to 1/L whilst bending frequencies are proportional to 1/L2. The Southwell-Dunkerly formula can then be used to combine the effects of both bending and shear deformations (of course both deformations have to occur in the same mode to be compatible) to obtain a frequency estimate as follows. 1 1 1 = 2 + 2 2 f n f n bending f n shear 314 Structural Engineering Analysis and Design Second Edition 4.1.3.4.3 Anisotropic Plate Simply-Supported The mode shapes are described by For mb = 1 (higher modes in this direction of much higher frequencies), the natural frequencies are Note only bending deformation accounted for; no shear deformation. The modal mass is then For MAX normalized mode shapes, the modal masses for ALL modes of the simply supported anisotropic plate are quarter of the total mass. Flat Slab Dx and Dy are flexural rigidity per unit width For unit width beam, the flexural rigidity, D = EI = Eh3/12 per unit width whilst for unit width plate, the flexural rigidity, D = EI = Eh3/[12(1-ν2)] per unit width. The torsional rigidity H should be such that it is equal to the bending rigidity D so that there is equal bending stiffness of the plate about any horizontal axis. The natural frequency of a square flat slab plate simply supported all round is f = 315 π a2 Eh 3 . 12m 1 − ν 2 ( ) Structural Engineering Analysis and Design Second Edition One-way Composite Spanning Two-way Composite Spanning Ribbed Section in One Direction y x Ribbed Section in Two Directions Dx is the flexural rigidity per unit width for bending about y-axis (or bending in x-z plane). Dy is the flexural rigidity per unit width for bending about x-axis (or bending in y-z plane); Iy = t.(H-h)3/12 + Aweb(lever arm)2 + (ay.h3/12)[ax/(ax-tortho+tortho.αortho3)] + Aslab(lever arm)2; Note the factor [ax/(ax-tortho+tortho.αortho3)] to account for the effect of the orthogonal ribs on the bending stiffness. Thus here αortho = h/Hortho where (Hortho h) is the depth of the orthogonal ribs and tortho is the thickness of the orthogonal ribs. 316 Structural Engineering Analysis and Design Second Edition 4.1.3.5 4.1.3.5.1 Approximate Formulae Multi-Storey Buildings A good approximate fundamental frequency formula for single-storey buildings, multi-storey buildings and towers is (Bachmann and EC1-2.4:1995) f = 46 / h (Hz) where h is the height (m). Alternatively, EC8 recommends for buildings up to 80m, where and Ct for structures with concrete or masonry shear walls is given by Another approximations is where 4.1.3.5.2 Cable Stayed Bridges A good approximate fundamental frequency formula for cable stayed bridges is (Bachmann) 317 Structural Engineering Analysis and Design Second Edition f = 110 / L where L is the length of the main span (m). 4.1.3.5.3 Highway Bridges A good approximate fundamental frequency formula for highway bridges is (Bachmann) f = 100 / L where L is the length of the main span (m). 318 Structural Engineering Analysis and Design Second Edition 4.2 GL, ML Implicit Direct Complex Modal (Eigenvalue) Analysis 4.2.1 Mathematical Formulation of Analysis The equation of motion for a free, damped system is [M ]{& u&( t )} + [C]{u&( t )} + [K ]{u ( t )} = {0} We seek solutions of the form [ {u(t)}i = Re al {φ}i ξ i e λ i t ] for the i th mode of vibration where ξ i = ξ Ri + iξ Ii and λ i = α i + iω di Note that α represents the decaying part and ω d the damped natural frequency. Hence, substituti ng into the equation of motion [M ]ξ i λ2i {φ}i e λ i t + [C]ξ i λ i {φ}i e λ i t + [K ]ξ i {φ}i e λ i t = {0} [λ [M] + λ [C] + [K]]{φ} 2 i i i = {0} This is a complex eigenvalue problem to be solved for λ i and {φ}i . For completion, the response due to mode i, {u(t)}i of a free damped linear elastic structure subjected to an initial impact (defining an initial displacement and velocity) is [ = {φ} Re al [(ξ = {φ} Re al [e {u(t)}i = {φ}i Re al ξ1i e λ1i t + ξ 2i e λ 2i t {u(t)}i {u(t)}i i i ] (cos ω di t + i sin ωdi t ) + (ξ 2 Ri + iξ 2 Ii )e α t (cos ωdi t − i sin ω di t )] αt [((ξ1Ri + ξ 2 R ) cos ωdi t − (ξ1Ii − ξ 2 Ii ) sin ω di t ) + i((ξ1Ii + ξ 2 Ii ) cos ωdi t + (ξ1Ri − ξ 2 Ri ) sin ω di t )]] 1Ri + iξ1Ii )e αi t i i For the free vibration response to be real for all t, and ξ1Ii = −ξ 2 Ii ξ1Ri = ξ 2 Ri Since there are two less independent constants, let ξ1Ii = −ξ 2 Ii = ξ Ii and ξ1Ri = ξ 2 Ri = ξ Ri We notice that ξ1i and ξ 2i are a complex conjugate pair ξ1i = ξ Ri + iξ Ii and ξ 2i = ξ Ri − iξ Ii Hence {u(t)}i = {φ}i e αi t (2ξ Ri cos ω di t − 2ξ Ii sin ω di t ) Thus the total response due to the superposition of all modes { } {u(t)} = [Φ ] e αi t (2ξ Ri cos ω di t − 2ξ Ii sin ω di t ) In the real eigenvalue analysis, for each mode i, NASTRAN outputs, one real root ω ni representing the undamped natural circular frequency one real eigenvector {φ}i representing the real mode shape Complex eigenvalue analysis with viscous (and structural optional) damping, for each mode i, NASTRAN outputs, two complex roots which are a complex conjugate pair, α i + iω di and α i − iω di , where α i is negative and represents the decaying constant ω di is positive and represents the damped natural circular frequency two complex eigenvectors which are a complex conjugate pair, {φ R + iφ I }i and {φ R − iφ I }i Complex eigenvalue analysis with only structural (and no viscous) damping, for each mode i, NASTRAN outputs, one complex root, α i + iω di , where α i is negative and represents the decaying constant ω di is positive and represents the damped natural circular frequency one complex eigenvector, {φ R + iφ I }i 319 Structural Engineering Analysis and Design Second Edition 4.2.2 Complexity of Modes of Vibration A pure real mode has all its terms in phase which each other. Different modes will of course be out of phase with each other, but every point in a particular mode will vibrate in phase. And so, for a mode, all points in the structure reach its maximum and minimum at the same phase instant. A complex mode on the other hand will have different points of the structure reaching its maximum at different phase instants, i.e. different points of the structure are out of phase with each other for a particular mode. Of course, different modes are still out of phase with each other. The degree to which these points are out of phase with each other is a measure of the complexity of the mode. An Argand diagram with all the terms of the complex eigenvector plotted will exhibit a narrowband if the mode is only slightly complex. The diagram below shows plots for 4 eigenvector terms. Since there is only a slight phase difference between the terms (angle between the arrows), the 4 terms define an almost real complex eigenvector. Im Re The following eigenvector plot on the other hand is highly complex because of the large phase angle difference between the terms of the eigenvector. Im Re The animation of the complex modes is quite indicative of the complexity of the mode. In complex modal analysis, each mode has two complex conjugate eigenvectors. Each eigenvector has a real and imaginary part. The animation of such a complex mode is only of value when we plot the magnitude of either (of the two complex conjugate) eigenvectors. The phase information (which is obtained when the magnitude and argument of the real and imaginary components are obtained) is essential in order to determine the relative phase of the motion of different parts of the structure. In a real mode, there is no phase information, and hence the animation of a real mode will show all parts of the structure vibrating in-phase with each other. Explicit viscous dampers will cause parts of the structure to vibrate clearly out-of-phase. This clearly occurs when explicit viscous dampers are used to damp prestressed cable vibrations. A cable with a damper element of a very high damping coefficient attached to its center will behave as two separate cables, the damper element effectively producing a fixity at the center of the cable. This changes the fundamental mode shape of the cable from one of a low frequency to two cable mode shapes of higher fundamental frequency. 4.2.3 Complex Modal Analysis To Determine Modal Damping Values Because the solution by complex modal analysis yields a decaying constant αi for each and every mode, the modal damping can be obtained as modal structural damping, Gi = 2αi/ωdi. 320 Structural Engineering Analysis and Design Second Edition 4.2.4 4.2.4.1 MSC.NASTRAN Decks GL, ML Complex Modal Analysis $ EXECUTIVE CONTROL SECTION SOL 107 $ CASE CONTROL SECTION $ Sets defining grid ids or element ids SET < Number > = 1 THRU 100, 211, 343, < etc > $ Grid output of displacement for each mode i.e. eigenvector $ SORT1 lists the results by eigenvalue whilst SORT2 lists the results by grid id DISPLACEMENT(,,) = ALL/ $ Grid output of displacement for each normalized mode i.e. normalized eigenvector SDISPLACEMENT(,,) = ALL/ $ Grid output of real eigenvector for the a-set SVECTOR() = ALL/ $ Grid output of SPC forces SPCFORCES(,,) = ALL/ $ Element output of force, stress and strain ELFORCE(,,) = ALL/ ELSTRESS(,,) = ALL/ STRAIN(,,) = ALL/ $ Analysis Requests SPC = < ID of SPC Cards Defined in Bulk Data > CMETHOD = < ID IN EIGC > $ XY plot output OUTPUT(XYPLOT) XYPUNCH RESPONSE /() XYPUNCH RESPONSE /() The EIGC bulk data card is required. The METHOD commonly used is CLAN. NORM, G, and C have to do with the specification of the method of normalization. The eigenvectors may be normalized either to a unit value at grid point G for coordinate C, or for the largest term to be of unit magnitude. E is used to specify the convergence criterion of the solution. Each method has a different default value for this criterion, and each is adequate for most problems. The following continuation is repeated for each desired search region. (J = 1 to n, where n is the number of search regions). As mentioned, replacing the following into the free damped equation of motion results in the following complex eigenvalue problem where 321 Structural Engineering Analysis and Design Second Edition If α=0, the radian frequency, ω of complex eigenvalue analysis is the same as that of real eigensolutions. The real part, α, is a measure of the decay rate of a damped structure, or if negative, the rate of divergence of an unstable system. The imaginary part, ω, is the modified frequency in radians/unit time. However, roots with negative values of ω should be treated as special terms. The recommended practice is to specify one point α1=0.0 and ω1 at the lower bound of the expected range of eigenvalues, but not at 0.0. A second shift may be input at α2=0.0 and ω2 at the upper bound of the expected range. All ALPHABj and OMEGABj must be blank. The eigenvalue output for a sample problem is shown below. The column labeled (REAL) contains α1, and the column labeled (IMAG) contains ω1. The column labeled (FREQUENCY) contains the circular frequency. The last column is the damping coefficient computed from the equation which is approximately twice the value of the conventional modal damping ratio. Note that if the magnitude of this term is computed to be less than 5.0x10-4, it is reset to zero. For small values, the damping coefficient is twice the fraction of critical damping for the mode. The eigenvalues are sorted on ω, with the negative values sorted first (there are none in this example), sorted on increasing magnitude, followed by the eigenvalues with positive ω, again sorted on magnitude. Roots with equal ω values are sorted next on α. 322 Structural Engineering Analysis and Design Second Edition 4.2.4.2 GL, ML P-∆ (KGA From KEA) Complex Modal Analysis It is often necessary to incorporate the reduction in bending stiffness of gravity load resisting columns for the analysis of lateral loads. The following procedure is undertaken. Phase 1 Perform static analysis (with loads that cause the greatest negative or positive geometric stiffness) based on [KEA] but include the segyroa.v2001 alter prior to the Case Control Section in order to compute the geometric stiffness matrix [KGA]1 (and output into a .pch file) based on the generated element loads from the [KEA] static analysis. Phase 2 A SOL 107 is undertaken based on [KEA] + [KGA]1 with the k2gg=ktjj statement in the Case Control Section and the outputted .pch file which contains the ktjj matrix in the Bulk Data. The responses at this stage represent the P-∆ (KGA From KEA) complex modal response. The following equivalent alternative procedure can also be employed. $ CASE CONTROL SECTION SUBCASE 1 LABEL = Static Preload Load Case LOAD = < ID of FORCEi, MOMENTi, PLOADi, GRAV, LOAD, SPCD Cards in Bulk Data > TEMP(LOAD) = < ID of TEMP, TEMPRB, TEMPP1 Cards in Bulk Data > DEFORM = < ID of DEFORM Cards in Bulk Data > SUBCASE 2 LABEL = P-∆ Complex Modal Analysis STATSUB(PRELOAD) = 1 CMETHOD = < ID in EIGC > The method is valid when only the prestress is judged to affect the geometric stiffness such as in the compressive preload of building columns due to gravitational loads and the prestressing of extremely taut cables that sag very little under gravity but not in systems such as suspension bridges. Where lateral loads are large enough to affect the geometry of the system with prestress, then a repetitive P-∆, SOL 106, implicit dynamic relaxation SOL 129 or explicit dynamic relaxation must be employed. But in single P-∆ analysis, because cables do not have much elastic bending stiffness, the initial static preload subcase should only include the prestress and not gravity as including gravity is the same as solving two linear static problems of stiffness KEA with preload and gravity as the applied loads respectively. Clearly, in the gravity case, it is nonsensical as the cables do in reality have differential stiffness (from the prestress) to resist the gravitational force. Prestress in one direction (i.e. along the axis of cable) will cause a differential stiffness in the orthogonal direction. Gravity acts in the orthogonal direction and hence cannot be accounted for in the calculation of the prestress in this single P-∆ analysis. To quantitatively decide if gravity need not be considered in contributing to the differential stiffness of the cables, a static P-∆ analysis should be carried out, the first subcase being a SOL 101 with only the prestress as applied loads and the second subcase a P-∆ SOL 101 (i.e. utilizing the induced prestress from the first subcase to form a geometric stiffness matrix) with both the gravity and prestress included as applied loads. If the difference in the cable element forces between subcases 1 and 2 is negligible, then gravity has little influence in affecting the geometric stiffness. If there is a major difference in the cable element force, then clearly, gravity will affect the geometric stiffness and as such, a repetitive P-∆ , SOL 106, implicit dynamic relaxation or explicit dynamic relaxation must be used to converge to the true KT. Likewise, in the single P-∆ analysis of multi-storey buildings, gravity (and only gravity) acts in axis of columns to generate prestress, and the differential stiffness is computed for the orthogonal direction reducing resistance to lateral wind forces, applied in the second subcase with gravity too. 323 Structural Engineering Analysis and Design Second Edition The STATSUB(PRELOAD) computes the differential stiffness due to the prestress and also the follower force. The follower force is calculated and incorporated by the use of PARAM, FOLLOWK, YES. We know how the prestress affects the differential stiffness, namely a tensile prestress causing an increase in stiffness. The effect of the follower force on the stiffness is different. For example, for a cylinder under external pressure critical buckling load may be overestimated (even though the mode shapes are similar) in a SOL 105 and the natural frequencies in vibration may be underestimated (even though the mode shapes are similar) in a SOL 103 in the absence of follower stiffness. To the contrary, these observations are reversed in case of centrifugal loads. Centrifugal forces as a constant (static) load are applied by a Bulk Data RFORCE to any elements that have masses. The follower stiffness due to centrifugal load has the effect of lowering stiffness (although the centrifugal load tensioning effect increases stiffness), consequently lowering natural frequencies (even though the mode shapes are similar) in a SOL 103 and lowering the buckling loads (even though the mode shapes are similar) in a SOL 105. This effect increases as the RPM increases, and it becomes significant when the RPM is over 1000. For moderately geometric nonlinear analysis, exclusion of follower stiffness affects the rate of convergence, but the converged solution is correct. For severely geometric nonlinear analysis, it may not be possible to obtain a converged solution without including follower stiffness. As the geometric nonlinearity intensifies, so is the effect of follower stiffness. Therefore, inclusion of follower stiffness greatly enhances the convergence if the deformation involves severe geometric nonlinearity. 324 Structural Engineering Analysis and Design Second Edition 4.2.4.3 GL, ML P-∆ (KGA From Exact or Approximate KTA) Complex Modal Analysis The above top deck solves the linear modal complex eigenvalue problem. It is often necessary to include the differential stiffness, especially if there are prestressed cables in the model and the mode shapes are sought. To obtain KTA, to be theoretically exact, a GNL SOL 106 (or implicit dynamic relaxation SOL 129 or explicit dynamic relaxation LS-DYNA) with prestress (as temperature loads say) and gravity must be undertaken. Alternatively, an approximation to KTA can be obtained by repetitive P-∆ static analyses with the prestress (as temperature loads say) and gravity applied. The procedure to obtain this approximate KTA will be presented. Note that the approximate KTA will be the summation of the elastic stiffness KE at the undeflected (by the prestress and gravity) state but KG at the deflected (by the prestress and gravity) state. Hence if KE changes considerably during the application of the prestress, a full SOL 106 (or implicit dynamic relaxation SOL 129 or explicit dynamic relaxation LS-DYNA), which converges to the KE and KG at the deflected (by the prestress and gravity) state should be employed. Hence for the modelling of a suspension bridge where there is a great change in geometry (known in the bridge industry as form-finding, so-called because it is necessary to find the form or shape of the catenary suspension cables), it may be prudent to employ SOL 106 (or implicit dynamic relaxation SOL 129 or explicit dynamic relaxation LSDYNA), but for a high tension low sag cable on say a tower with prestressed cables, the repetitive P-∆ static analysis may be adequate. The repetitive P-∆ analysis basically involves a number of iterations of linear static analyses to obtain an approximate KTA. Note again that A refers to the initial undeflected (by the collapsing load) state, but deflected by the prestress and gravity. To perform the repetitive P-∆ analysis, a static analysis is performed based on KEA with temperature loads and gravity to generate forces in the structural elements, which in turn provides input for the computation of KGiAKTm where m is the iterations. Repetitive static analysis is performed with the prestress and gravity updating the stiffness matrix KEA + KGiAKTm-1 + KGiAKTm until convergence of displacements is obtained. The tangent stiffness at this stage is the approximate converged tangent stiffness matrix KTA = KEA + KGiAKT. The converged displacements represent the approximate P-∆ (KGA From Approximate KTA) static response to the initial prestress loads. The converged geometric stiffness at this stage would be that based upon the approximate tangent stiffness matrix KTA, i.e. KGiAKT. Phase 1 Perform static analysis (with prestress and gravity) based on [KEA] but include the segyroa.v2001 alter prior to the Case Control Section in order to compute the geometric stiffness matrix [KGA]1 (and output into a .pch file) based on the generated element loads from the [KEA] static analysis. Phase 2 Perform static analysis (with prestress and gravity) based on [KEA] + [KGA]1 by including the k2gg = ktjj statement in the Case Control Section, the outputted .pch file which contains the ktjj matrix in the Bulk Data and the segyroa.v2001 alter prior to the Case Control Section to compute the [KGA]2 (and output into the .pch file overwriting previous data) based on the generated element loads from the [KEA] + [KGA]1 static analysis. Phase 3 Repeatedly perform the Phase 2 static analysis (with prestress and gravity) based on [KEA] + [KGA]i for i = 2 to n where n represents the number of iterations required for the change in deflections between analyses to become negligible. This would signify that the change in the [KGA] matrix become negligible and the correct [KGA] is attained. The deflections and the other responses at this stage represent the P-∆ (KGA From Approximate KTA) static response to the prestress and gravity. The stiffness of the structure is KTA. Phase 4 A SOL 107 is undertaken with the k2gg=ktjj statement in the Case Control Section and the outputted .pch file which contains the latest ktjj matrix in the Bulk Data. The responses at this stage represent the P-∆ (KGA From Approximate KTA) complex modal response. 325 Structural Engineering Analysis and Design Second Edition 4.2.5 4.2.5.1 Hand Methods Verification Determination of Damped Natural Frequency and the Maximum Dynamic Displacement, umax for Free Damped Vibration Due to Initial Displacement and/or Initial Velocity by Classically Solving the SDOF Linear ODE and Maximizing the Solution Equation of motion (linear second order ODE) m& u&( t ) + cu&( t ) + ku ( t ) = 0 [ ] Assume u(t) = Re al Ge λt where G = G R + iG I and λ = α + iω d 2 λt mGλ e (mλ + cGλe λt + kGe λt = 0 ) + cλ + k Ge λt = 0 for LHS to be zero for all t 2 (mλ 2 ) + cλ + k = 0 Ge λt > 0 as the roots of this quadratic characteristic equation are 2 2 c k c k  c   c  +  λ2 = − −   −  − 2m m 2m m  2m   2m  Hence the general solution is the superposition of the two possible solutions, λ1 = − [ u(t) = Re al G 1e λ1t + G 2 e λ 2 t ] The exact form depends on the value of the viscous damping coefficient, c. Case : critically damped c = c cr = 2 km = 2mω n , the two roots are real and repeated, λ1 = λ 2 = − c cr 2 km =− 2m 2m Hence, u(t) = (G 1 + G 2 t )e − c cr t 2m There will be no oscillatory motion, instead simply an exponentia l decay. Case : overdamped c > c cr , the two roots will be real and distinct, u(t) = G 1e λ1t + G 2 e λ 2 t Again, there will be no oscillatory motion, instead exponential decay in a longer time. 326 Structural Engineering Analysis and Design Second Edition Case : under - damped, c < c cr , the roots are complex conjugates , c k  c  +i −  2m m  2m  employing Euler' s equations, 2 λ1 = − λ2 = − c k  c  −i −  2m m  2m  2 e iθ = cos θ + i sin θ e −iθ = cos θ − i sin θ k  c  −  m  2m  hence, writing ωd = 2 c c   t t − − u ( t ) = Re al (G 1R + iG 1I )e 2 m (cos ωd t + i sin ωd t ) + (G 2 R + iG 2 I )e 2 m (cos ωd t − i sin ω d t )    −ct  u ( t ) = Re al e 2 m [((G 1R + G 2 R )cos ωd t − (G 1I − G 2 I )sin ωd t ) + i((G 1I + G 2 I )cos ω d t + (G 1R − G 2 R )sin ω d t )]   for the free vibration response to be real for all t, G 1I = −G 2 I G 1R = G 2 R and sin ce there are two less independen t constants, let G 1I = −G 2 I = G I and G 1R = G 2 R = G R we notice that G 1 and G 2 are a complex conjugate pair G 1 = G R + iG I and G 2 = G R − iG I hence u(t) = e − c t 2m [(2G R cos ωd t − 2G I sin ωd t )] defining the damping ratio ζ such that c = ζc cr = ζ 2 km = ζ 2mω n the damped natural circular frequency, ωd = k  ζ 2 km − m  2m 2   =   k ζ2k − = m m ( ) k 1 − ζ 2 = ωn 1 − ζ 2 m hence, u ( t ) = e −ζωn t [(2G R cos ωd t − 2G I sin ωd t )] where ωd = ω n 1 − ζ 2 and 2G R , − 2G I being the constants of integratio n from the initial conditions . Note also that we often define the decaying constant c 2m hence since c = ζ 2mω n α=− ζ 2 mω n 2m α = −ζω n α=− 327 Structural Engineering Analysis and Design Second Edition Damping causes the damped natural frequencies to be a little less than the undamped natural frequencies, but the difference is negligible in real structures, which are under-damped. Hence, the old classroom example of measuring the natural frequency of a pendulum in air and in water gives a lower frequency in water simply because of the added water mass in the dynamic model. We have established that for under - damped free vibrations u ( t ) = e −ζωn t [(2G R cos ωd t − 2G I sin ωd t )] With initial displacement and velocity conditions,   u&(0) + u (0)ζω n u ( t ) = e −ζωn t  u (0) cos ωd t + sin ωd t  where ωd = ω n 1 − ζ 2 ωd   Hence, the maximum dynamic displacement u max  u&(0) + u (0)ζω n = u (0) +  ωd  2    2 The motion is oscillatory with a period of Td = 2π , the amplitude decreasing exponentially. ωd The damping ratio ζ can be estimated experimentally from two displacement peaks separated by mTd , 2π ζω m 2π ζm 2π 2 πζm n ζωn m 2 2 un e −ζωn t1 ωn 1−ζ 2 ωd = −ζω ( t + mT ) = e ζωn mTd = e =e = e 1−ζ = e 1−ζ n 1 d u n+m e The logarithmic decrement is defined as the natural log of the ratio between successive peaks (m = 1), δ = ln un 2πζ = ≈ 2πζ u n +1 1− ζ2 328 Structural Engineering Analysis and Design Second Edition 4.3 4.3.1 GL, ML Implicit (Real) Modal Frequency Response Analysis Nature of the Dynamic Loading Function The solution method can be used to solve dynamic systems subjected to: (a) Deterministic periodic harmonic long duration loading functions A deterministic periodic forcing function has regularly repeating amplitude. The sine or cosine function is said to be harmonic. Because the periodic function repeats itself, any initial starting transient response is insignificant and the steady state response is of interest, hence the solution is performed in the frequency domain. The starting transient normally decays away after 50-100 cycles of oscillation for light damping. The steady-state oscillatory response occurs at the same frequency as the loading phase shifted due to damping. In this LINEAR FREQUENCY DOMAIN solution, not only that the static response has to be added separately, but also the mean of the dynamic excitation has also got to be added separately as a static response. This is because the mean of the dynamically applied force is not included in the dynamic excitations. Hence the total response in this frequency domain dynamic analysis = static response to mean of dynamic excitation + dynamic response + static response to static loads. 4.3.2 Mathematical Formulation of Analysis In the modal frequency analysis, the solution of a particular forcing frequency is obtained through the summation of the individual modal responses. With the knowledge of the modal frequencies and corresponding mode shapes, the coupled system of simultaneous dynamic equilibrium equations can be uncoupled by premultiplying the dynamic equation of motion by [Φ]T as shown below. This means that the simultaneous ODEs no longer need to be solved simultaneously and so the MDOF system of equations is reduced to a SDOF system of equations, which can be solved independently of each other. The computational benefit comes from not having to run a rigorous simultaneous equation solver. The knowledge of the modal frequencies and the corresponding mode shapes are a prerequisite to this implicit modal frequency response analysis, hence the implicit real (note not complex) eigenvalue analysis must be performed first. Because of the fact that the modes are real and do not take into account the explicit elemental (structural and viscous) damping within the structure, the coupled ODEs cannot be uncoupled by [Φ]T. The system of coupled ODEs remains in the existence of structural and/or viscous damping and the simultaneous equation solver must be invoked. The only difference then between SOL 111 and SOL 108 is the fact that the former solves the equations in the modal coordinates instead of the physical coordinates. Hence, as long as sufficient modes are included (to represent both the static and dynamic response of the system), SOL 111 will give the same solution as SOL 108 even with large values of structural and/or viscous damping. We know that large values of elemental damping will modify the mode shape and frequencies. However, a SOL 111 can still be performed because a true (real) modal approach is not undertaken, instead the coupled ODEs are solved using a direct approach, but in the modal coordinates. However, the use of the FREQ4 card, which bases the excitation frequencies to be solved for on the real natural frequencies may prove to be insufficient. This is because with high values of elemental viscous damping, certain local modes can be totally eliminated. For instance, viscous dampers with high coefficients of damping on cables can considerably alter the natural frequency of the local mode and even eliminate a local mode altogether. In this case, the FREQ4 card will not capture the response at the damped natural frequency. Hence, these damped natural frequencies need to be known (by performing a SOL 107) before choosing the excitation frequencies to be solved for using FREQ2 cards. To reiterate, SOL 111 reverts to a direct solution technique (akin to SOL 108) when there is either viscous or structural element damping as the equations of motion cannot be orthogonalized. But the unknowns are still the modal responses and not the physical responses. And because with damping the modes are really complex modes, there is greater difficulty in capturing all the response using the real modes. Hence, even more modes are thus required to capture the response accurately in SOL 111 with element damping especially if the elemental damping is high enough to cause significant complex modes. Thus if elemental damping is high and the modes are complex, the direct method SOL 108 may be more appropriate. If a true modal approach is intended for the solution of coupled ODEs with structural and/or viscous damping, then a complex modal forced frequency response analysis is necessary, although this is quite impractical. 329 Structural Engineering Analysis and Design Second Edition The modal matrix from the free, undamped modal analysis is [Φ ] = [{φ}1 ... {φ}i ... {φ}n ] The coupled system of ODEs of the undamped forced vibration equation of motion is [M ]{& u&( t )} + [K ]{u ( t )} = {P( t )} In the frequency domain, let {u(t)} = Re al [[Φ ]{ξ(ω)}eiωt ] where {ξ(ω)}is a complex modal displacement response function vector {P(t)} = Re al [{P(ω)}e iωt ] where {P(ω)}is a harmonic loading function vector This transformation is worth a little explanation. The harmonic forcing function in the time domain P(t) is transformed into the frequency domain simply by multiplying {P( t )} = Re al [{P(ω)}e iωt ] {P(ω)} is the complex harmonic forcing function. The harmonic term is eiωt. {P(ω)} can be frequency dependent and/or can even be complex in general. If {P(ω)} is complex, this refers to harmonic loading functions which are out of phase with respect to each other. We usually assume that {P(ω)} is frequency independent and also just real, such that {P(ω)} = {p0}. The frequency domain complex forcing function {P(ω)} is specified in NASTRAN with the RLOAD1 and RLOAD2 cards. The harmonic term is inferred naturally. Note that in the modal approach of the response analysis, the complex modal response is ξi(ω) and that the total complex response function is F(ω). {F(ω)} = [Φ ]{ξ(ω)} It must be stressed that the specified frequency domain excitation is the complex harmonic forcing function {P(ω)} and that the corresponding complex total response vector is {F(ω)}. If {P(ω)} is complex, then {F(ω)} will be complex. If {P(ω)} is only real, than {F(ω)} will be real if there is no damping in the system but will be complex if there is damping in the system. The curves for {F(ω)} versus ω is what is produced by the NASTRAN output in a frequency domain analysis. It can be viewed in its real and imaginary components versus ω, or in its magnitude and phase versus ω, the latter of which is what should be observed to ascertain the response. To summarize Frequency domain loading function from the time domain loading function [ {P( t )} = Re al {P(ω)}e iωt ] where {P(ω)} is the complex loading function vector Frequency domain complex modal response to {P(ω)} is {ξ(ω)} which is complex in general Frequency domain complex total response function vector {F(ω)} = [Φ ]{ξ(ω)} where {F(ω)} is complex in general Time domain total response from the frequency domain complex total response [ {u ( t )} = Re al {F(ω)}e iωt ] 330 Structural Engineering Analysis and Design Second Edition We have specified that {u ( t )} = Re al [[Φ ]{ξ(ω)}e iωt ] This transforms the physical coordinates {u(ω)} to modal coordinates {ξ(ω)}. The mode shapes [Φ ] are used to transform the problem in terms of the behavior of the modes as opposed to the behavior of the grid points. This equation represents an equality if all the modes are used, but since all the modes are rarely used, the equation usually represents an approximation. Hence, the equation for harmonic motion in terms of the modal coordinates is −[M ][Φ ]{ξ(ω)}ω 2 e iωt + [K ][Φ ]{ξ(ω)}e iωt = {P(ω)}e iωt −ω 2 [M ][Φ ]{ξ(ω)} + [K ][Φ ]{ξ(ω)} = {P(ω)} Premultiplying by [Φ ]T reduces the coupled system of ODEs to a system of uncoupled ODEs −ω 2 [Φ ]T [M ][Φ ]{ξ(ω)} + [Φ ]T [K ][Φ ]{ξ(ω)} = [Φ ]T {P(ω)} −ω 2 [M]{ξ(ω)} + [K ]{ξ(ω)} = {P(ω)} where the diagonal generalised (modal) mass matrix, [M] = [Φ ]T [M ][Φ ] [ ] the diagonal generalised (modal) stiffness matrix, [K] = [Φ ]T [K ][Φ ] = ω n 2 [M] the generalised (modal) force vector, {P(ω)} = [Φ ] {P(ω)} The matrices [M] and [K] are diagonal because of the orthogonality condition of the normal modes T {φi }T [M ]{φ j } = 0 and {φi }T [K ]{φ j } = 0 if i≠ j Accordingly, the generalised mass solitary term and the generalised stiffness solitary term associated with a particular mode ' i' are M i = {φ i } [M ]{φ i } T and K i = {φ i } [K ]{φ i } = ω 2ni M i T And because these matrices are diagonal, the equations become uncoupled and is easy to solve for {ξ(ω)}. Hence, the set of uncoupled SDOF systems is −ω 2 M i ξ i (ω) + K i ξ i (ω) = Pi (ω) ξ i (ω) = Pi (ω) − ω 2Mi + K i for i = 1 to n modes which is solved for the individual modal responses ξ i (ω). Finally, the total physical response is the superposition of the individual modal responses {u ( t )} = Re al [[Φ ]{ξ(ω)}e iωt ] {u ( t )} = Re al [{F(ω)}e iωt ] In modal frequency response analysis, mode truncation refers to not utilizing all the natural modes in computing the response of the structure. At a minimum all the modes that have resonant frequencies that lie within the range of the forcing frequencies have to be retained. For better accuracy, all the modes up to at least 2 to 3 times the highest forcing frequency should be retained. For example, if a structure is excited between 200 and 2000 Hz, all modes from 0 to at least 4000 Hz should be retained as the forcing frequencies still excite the higher modes although not resonating with them, i.e. off-resonant excitation. The recommendation of using modes up to 2 or 3 times the highest excitation frequency assumes that the static response can be captured adequately using this finite number of modes. Clearly, if the distribution of applied loads is multiple concentrated forces, then the finite number of modes may still not be sufficient to capture the difficult static shape. In this case, it may be prudent to use static residual vectors instead of increasing the number of vibration modes solely to capture the static response. 331 Structural Engineering Analysis and Design Second Edition The following damping models are supported by the solution scheme I. elemental damping i. viscous damping Yes ii. structural damping Yes II. modal damping i. viscous damping Yes ii. structural damping Yes III. global proportional viscous damping i. mass proportional damping No ii. stiffness proportional damping Yes iii. Rayleigh damping No If explicit viscous damping element contributions are made to the damping matrix [C] or if elemental structural damping is specified such that a complex stiffness matrix exists, then neither the damping nor the stiffness matrices can be diagonalized by the modal matrix. In this case the modal frequency response analysis solves the still coupled problem using a direct frequency approach but in terms of the modal coordinates {ξ(ω)} instead of the physical coordinates {u(t)}. Since the number of modes used in a solution is typically much less than the number of physical variables, using the coupled solution of the modal equations is less costly than using physical variables. Hence, with elemental viscous and/or elemental structural damping, the coupled system of ODEs of the damped harmonically forced vibration equation of motion is given by [M ]{& u&( t )} + [C ]{u&( t )} + [ K ]{u ( t )} = {P ( t )} where [ K ] = (1 + iG )[ K ] + i [C ] = Hence, ∑ [C E ∑G E [K E ] ] [− ω [Φ ] [M ][Φ ] + iω[Φ ] [C][Φ ] + [Φ ] [K ][Φ ]]{ξ(ω)} = [Φ ] {P(ω)} 2 T T T T The modal frequency response analysis solves the still coupled problem using a direct frequency approach but in terms of the modal coordinates {ξ(ω)} instead of the physical coordinates {u(t)}. If however only viscous modal damping ζi is specified, the generalized damping matrix [Φ]T[C][Φ] remains diagonal and so the uncoupled equations of motion can be maintained. The uncoupled equations of motion become −ω2Mi ξ i (ω) + i(ζ i 2Mi ω n i )ωξ i (ω) + K i ξ i (ω) = Pi (ω) ξ i (ω) = for i = 1 to n modes Pi (ω) − ω2Mi + i(ζ i 2M i ωn i )ω + K i which is solved for the individual modal responses ξ i (ω). The animation of the forced frequency response is quite indicative of the nature of the response of the structure to harmonic excitations. The forced frequency response analysis will yield for each node, both real and imaginary responses. The animation of the forced response of the structure as a whole (at any particular frequency of excitation) is only of value when we plot the magnitude of the response, and not the individual real or imaginary components. The phase information (which is obtained when the magnitude and argument of the real and imaginary components are obtained) is essential in order to determine the relative phase of the motion of different parts of the structure. Explicit viscous dampers will cause parts of the structure to vibrate clearly out-of-phase. 332 Structural Engineering Analysis and Design Second Edition If only structural modal damping Gi is specified, modal damping is processed as a complex stiffness of each individual mode and so the uncoupled equations of motion can still be maintained. The uncoupled equations of motion become −ω2Mi ξ i (ω) + (1 + iG i (ω)) K i ξ i (ω) = Pi (ω) ξ i (ω) = for i = 1 to n modes Pi (ω) − ω2M i + (1 + iG i (ω)) K i which is solved for the individual modal responses ξ i (ω). It is important to know how to convert between structural damping and equivalent viscous damping for a particular mode. For a particular mode, Viscous damping, Fviscous = ζ i (critical damping) (mod al velocity) = ζ i (2Mi ωn i ) (iωξi {φi }) Structural damping, Fstructural = iG iK i ξi {φi } For the two forms to be equal, Fviscous = Fstructural ζ i (2Mi ωn i ) (iωξi {φi }) = iG iK i ξi {φi } In the special case that ω = ωn i ζ i (2Mi ωn i ) = G iK i 2 ζ i (2MiK i / Mi ) = G iK i 2ζ i = G i Hence, the relationship Gi = 2ζi can be used to specify an equivalent viscous damping for structural damping, but is only exact when the forcing frequency ω = the natural modal frequency ωni which occurs at resonance, i.e. when damping is of primary importance. The complex response function due to a loading {P(ω)} is defined as {F(ω)} = −ω 2 {P(ω)} [M ] + iω[C] + [K ] The complex transfer function is defined as the complex frequency response function due to unit harmonic excitations [H(ω)] = 1 − ω [M ] + iω[C] + [K ] 2 This is the so-called transfer function that transfers the excitation to the response as follows [ {u ( t )} = Re al [H (ω)]{P(ω)}e iωt ] The (magnitude of the) dynamic amplification function D(ω) is defined as the magnitude of the complex response function {F(ω)} divided by the static displacement. 333 Structural Engineering Analysis and Design Second Edition 4.3.3 Capability of A Finite Number of Modes To Model The Static and Dynamic Response of Structure When running a modal based dynamic response analysis, it is imperative to know if the chosen number of modes within the modal dynamic analysis is capable of representing both the static and dynamic response of the structure. First and foremost, the chosen modes must cover and extend beyond the excitation frequency range such that both the resonant response of the modes within the range and the off-resonant response of the modes beyond (from say a 1/3rd of lowest excitation frequency to 3x the highest excitation frequency) the range are captured. This will sufficiently model the dynamic response. Considerations then must be made for the finite number of modes to capture the static response. It is often said in dynamic analyses that if the chosen finite number of modes are capable of representing the static response, then they will usually also be able to represent the dynamic response of the structure. We shall consider the frequency domain as this enables us to plot the FRF (and hence of course also the transfer function and the dynamic amplification function). Let us picture the (magnitude of the) dynamic magnification function, here shown below for a single mode, i.e. a SDOF system. Damping Controlled Inertia Controlled D Stiffness Controlled Dmax ≈ Dresonant = 1/(2ζ) 0 ω ωn 1 The finite number of modes should be able to represent the true static displacement at zero excitation frequency and the maximum (magnitude of the) dynamic amplification. Obtaining just the correct maximum (magnitude of the) dynamic amplification is not proof that the chosen finite number of modes is sufficient. This is because the response D(ω) at the frequency corresponding to the maximum dynamic response is controlled only by the damping within the structure. Note that the corresponding value F(ω) is also a function of the modal stiffness (or modal mass), the natural frequency and the (amplitude of the) modal force. Hence if the static response is inaccurate, so will be the dynamic response. Thus it is best to compare the response function F(ω) between the modal model and the full MDOF model. To compare individual components of the modal model, the following approach is undertaken. First, the accuracy of the stiffness representation is investigated. This corresponds to the static displacement. When the excitation frequency is zero, if the modal approach with SOL 111 achieves the same F(ω) response as that from a static analysis SOL 101, then the chosen finite modes are capable of representing the stiffness within the system and hence are capable of modelling the static response for the system. The mathematics of converting the static equilibrium equations in physical coordinates to equations in modal coordinates (and hence with a certain degree of modal truncation unless the number of modal coordinates equals the number of physical coordinates) is presented in Section 3.1.4. Thereafter, the damping representation is evaluated by comparing the response F(ω) at the frequency of maximum amplification. Finally, the inertial representation is evaluated by comparing the response F(ω) at high excitation frequencies. If the responses obtained from the modal approach when the excitation frequency is off-resonant is similar to that obtained from the multi degree of freedom model, then the chosen finite number of modes are capable also of modelling the mass and stiffness distribution within the system. 334 Structural Engineering Analysis and Design Second Edition Hence, in order to quantitatively decide whether the chosen number of finite modes is capable of representing a multi degree of freedom system the response between a direct solution SOL 108 and the modal solution SOL 111 is compared. The complex frequency response function F(ω) can be plotted for the response at the DOF of interest from both a SOL 108 and a SOL 111. A XYPLOT showing the contribution of individual modal responses F(ω) superposed on a plot containing the total physical response is most useful in visually determining the contribution of each and every mode to the static and dynamic response at particular frequencies of excitation. In MSC.NASTRAN, it is possible to plot the response function F(ω) for individual natural modes using SOL 111 (even if there is structural and/or viscous damping as SOL 111 then performs a coupled ODE solution process, but with the unknowns as the modal responses instead of the physical responses) by delimiting the mode calculated using EIGRL or using LFREQ (lower limit of the frequency range), HFREQ (upper limit of the frequency range) or LMODES (number of lowest modes retained). Alternatively, selective modes which are not sequential can be deleted by the user by using the alter delmodea.v2001 and the associated bulk data entry DMI. The degree of similarity between the two traces is an indication of the ability of the finite number of modes to represent the response of the system. The number of modes should be increased or decreased accordingly. Note that the static response at zero excitation frequency obtained from both SOL 111 and SOL 108 can be compared with the true static solution from a SOL 101. It will be found that SOL 108 will yield the same static response as SOL 101 (when there is no structural damping within the finite element model) whilst SOL 111 will yield a result that is lower due to the nature of the finite number of modes presenting a stiffer response. Incidentally, since SOL 108 does not allow the automatic specification of the frequency points to correspond to the natural frequencies of the structure, the user would have to perform a SOL 103 and manually specify to increase the resolution near the vicinity of the natural frequencies. It is essential that the sufficient modes be incorporated when derived quantities are intended. For instance, to evaluate the modal damping of a particular mode, both the static response and the dynamic response must be accurately represented. If the static response is not sufficiently captured, then the dynamic response will not be accurate either as the response of the FRF = P/K times D(ω). If the distribution of the excitation force is concentrated at multiple points, then it is likely that the difficult static shape requires many modes of vibration. In this case, it may be better to utilize static residual vectors to capture the response more directly. Alternatively of course, the direct frequency approach SOL 108 may be used, in which case the static response and the dynamic response of all modes are automatically captured, but it requires effort in capturing the peak response (by requesting fine frequency intervals near the peaks). But when using the modal method, damping estimates using the half power bandwidth on the FRF of the D(ω) or using 1/(2ζ) on the D(ω) depend on the capability of the modes to accurately represent the static and dynamic response. Where in doubt, use a SOL 101 solution to check the static response. And a SOL 107 solution should be used to check the modal damping estimates. The relative contribution of each mode to the total static and dynamic response can also be determined. This is known as the modal responses, i.e. the value of the modal variables in the modal solution scheme. The Case Control Cards SDISP, SVELO and SACCE will produce the modal solution set output, {ξi(ω)}. These are plots of the modal response (for each mode) in terms of frequency of excitation, i.e. the frequency domain modal response. That is to say, SDISP(PUNCH) (or SVELO or SACCE) will output one value for each mode at each excitation frequency. These are the modal responses in modal space. They must be multiplied by the corresponding mode shapes in order to obtain the modal responses in physical space i.e. {Fi(ω)} = {φi}ξi(ω) Another method of determining the modal contribution of individual modes to a particular excitation is by using the modal strain energy. Firstly, to evaluate the ability of the natural modes to represent the static response, a SOL 101 is run with the amplitude of the dynamic loads applied as a static load and the results are written to a DMIG file using the alter pchdispa.v2001. Then a SOL 103 us run with the DMIG included and also the alter modevala.v2001 to ascertain how well each and every mode can represent the static solution. The strain energy for each mode can be compared to the strain energy in all the modes calculated and also the input vector. Note that the eigenvector scaling must be set to the default MASS (not MAX) for this alter to be valid. Secondly, to evaluate the ability of the natural modes to represent the dynamic response, the alter mfreqa.v2001 is utilized for SOL 111. The results are presented in a matrix of strain energies with the rows representing the excitation frequencies and the columns 335 Structural Engineering Analysis and Design Second Edition representing the natural modes. The frequency interval between the rows and between the columns corresponds to the excitation frequency interval and the natural mode frequency interval. Of course, the dominant modes that represent the static response is not necessarily the same as the dominant modes that represent the dynamic response at different excitation frequencies. This is simply because the dynamic response is also a function of the loading frequency and resonance frequency, on top of the static response. Including the dominant modes that represent the static response will however improve the accuracy of representing the dynamic response F(ω) as it is the function of the amplification D(ω) and the static response P/K. Note that the capability of a finite number of modes to represent the static and dynamic response of the structure is limited to a particular force excitation direction and distribution. If the force changes its location or direction, then the prominence of the different modes which will be different. This is simply because changing the location or direction of the force will cause a different set of modal forces and hence a different level of excitation of the different modes. The capability of a finite number of modes to represent the static and dynamic response of the structure depends also on the level of elemental structural and elemental viscous damping present within the system. This is because, the level of elemental damping affects the complexity of the modes, hence possibly requiring more real modes if the modal complexity is high. Thus damping should be included when performing the study to determine the required number of modes. For accurate results of modal methods, static residual vectors (PARAM, RESVEC, YES) can be calculated except when using the seismic large mass method for enforced motion. The residual vector method is more efficient than the mode acceleration method and can be applied to both superelements and the residual structure when substructuring is employed. Clearly though, there should be sufficient modes comfortably beyond within the excitation frequency bandwidth to capture the dynamic response, and the static residual vectors should only be used as a final step to append the quasi-static responses of high frequency (relative to the excitation frequencies) modes. Note that SOL 111 reverts to a direct solution technique (akin to SOL 108) when there is either viscous or structural element damping as the equations of motion cannot be orthogonalized. But the unknowns are still the modal responses and not the physical responses. And because with damping the modes are really complex modes, there is greater difficulty in capturing all the response using the real modes. Hence, even more modes are thus required to capture the response accurately in SOL 111 with element damping especially if the elemental damping is high enough to cause significant complex modes. Thus if elemental damping is high and the modes are complex, the direct method SOL 108 may be more appropriate. Another method of determining the adequacy of the finite number of modes is to evaluate the cumulative effective mass of the chosen number of modes. The effective mass has got a specific meaning in seismic analysis, but can be used for other dynamic analyses as well as a measure of determining the adequacies of the finite number of modes. A cumulative effective mass that approaches unity suggests adequacy of the chosen modes to model the spatial distribution of the loading. This parameter of course does not say much about the adequacy of the chosen modes to model the frequency content of the loading. Essentially, and to reiterate, the chosen number of modes must be sufficient to model both the frequency content and also the spatial distribution of the loading. It is found that for a high cumulative effective mass, uniformly distributed loads such as in seismic analyses require only a few modes whereas a concentrated patch requires more modes and finally a highly concentrated load requires a much greater number of modes to capture the effect of the spatial distribution of the loading. 336 Structural Engineering Analysis and Design Second Edition 4.3.4 Complex Response F(ω) and Amplification D(ω) With Elemental and/or Modal Structural Damping The response at zero excitation frequency from a forced frequency response analysis (SOL 111 or SOL 108) will not be equal to the true static response (from a SOL 101 solution) if there is elemental or modal structural damping within the model. Intuitively, we know this to be true simply due to the fact that structural damping is independent of forcing frequency. Hence, there is no reason for it to be zero at an excitation frequency of zero. We shall illustrate this mathematically for modal structural damping although the same concept applies when there exist elemental structural damping. We know that the (magnitude of the) dynamic amplification factor for a mode when there is modal viscous damping is D i (ω) = (1 − ω 1 2 / ω ni ) 2 2 + (2ζ i ω / ω ni ) 2 If however we have modal structural damping, the modal equation of motion will be −ω 2 M i ξ i (ω) + i(ζ i 2M i ω n i )ωξ i (ω) + (1 + iG i ) K i ξ i (ω) = Pi (ω) ξ i (ω) = ξ i (ω) = Pi (ω) − ω M i + i(ζ i 2M i ω n i )ω + (1 + iG i ) K i 2 Pi (ω) − ω M i + i(C i ω + G iK i ) + K i 2 By complex arithmetic, we arrive to ξ i (ω) = (1 − ω Pi (ω) / K i 2 / ω ni ) 2 2 + (G i K i + 2ζ i ω / ω ni ) e − iθ i 2 And hence the (magnitude of the) modal dynamic amplification factor will be 1 D i (ω) = 2 2 2 1 − ω 2 / ω ni + (G iK i + 2ζ i ω / ω ni ) ( ) At zero excitation frequency, the (magnitude of the) dynamic amplification is thus not unity, but instead 1 D i (ω) = 2 1 + (G i K i ) As an aside, the (magnitude of the) dynamic amplification at resonance is D i (ω) = 1 G i K i + 2ζ i Thus, in general, with structural damping, the amplification at zero frequency is less than one simply due to the nature of structural damping being independent of excitation frequency. This should obviously not be the case for a true static solution since the static response is independent of damping. Hence, the response obtained at zero frequency from a forced response analysis of a system with structural damping is not the true static solution. This means that in order to derive the (magnitude of the) dynamic amplification function in a model with structural damping, it is necessary to perform a static solution SOL 101 to ascertain the actual static displacement and then divide the magnitude of the complex response function F(ω) from a SOL 108 solution by this value. 337 Structural Engineering Analysis and Design Second Edition 4.3.5 Representation of A MDOF System As A SDOF system A SDOF dynamic model is represented by a modal mass M, modal stiffness and modal damping. This SDOF model can even be modeled as a mass attached to a parallel spring and damper although hand calculations are sufficient to predict the response of a SDOF system exactly. The natural frequency is a function of the modal mass and modal stiffness. The modal masses, modal stiffnesses (or natural frequencies) of a MDOF system can be obtained from a real eigenvalue analysis SOL 103 or a back calculation from a SOL 111 analysis. The modal damping can be obtained from a complex modal analysis SOL 107. It will be shown that modes with small values of modal damping can be approximated simply as real modes (without its imaginary component). Hence, a real modal mass can be used. If however, the mode includes larges values of modal damping, its complex modal mass must be evaluated and subsequently a complex modal forced response analysis must ensue. Estimation of Real Modal Mass From A Forced Frequency Response Analysis Back-Calculation On A System Without Any Form of Damping This procedure is shown just to illustrate the dynamic response function. It is certainly as easy to obtain the modal mass from a real eigenvalue analysis. To determine the modal mass from a forced response back-calculation, the following procedure is undertaken. We know that P D(ω) K P P Hence, the static displacement = = 2 K ω M F(ω) = In order to compute the modal mass from a back-calculation of the forced response analysis, a SOL 111 should be performed with EIGRL limiting the calculated modes to only that being considered. Then the relationship above can be used to estimate the modal mass. Note that the static displacement obtained will be due only to the eigenvector being considered. The modal mass obtained using this method will correspond exactly to that calculated from Modal Mass, Mi = {φi}T[M]{φ i} Modal Mass of Modes With Small Values of Damping We know that P D(ω) K P P Hence, the static displacement = = 2 K ω M F(ω) = This shows that the modal mass is a function of the static displacement and not the (magnitude of the) dynamic amplification at resonance. At resonance, only damping controls the (magnitude of the) dynamic amplification response D(ω) of the structure. It is however, not true to say that the dynamic response F(ω) is controlled just by damping as it is also a function of the modal stiffness (or modal mass). At off-resonant frequencies stiffness, damping and inertia effects become prominent. The static displacement of the structure with or without damping in reality will be the same as long as elemental damping does not significantly alter the mode shape. At zero frequency of excitation, damping in reality does not affect the response because there are no dynamic effects. Hence, from the equation above, it becomes apparent that the modal mass M does not change as long as the natural frequency of the mode does not change significantly. As a rule, as long as the mode shapes and the natural 338 Structural Engineering Analysis and Design Second Edition frequency does not change too much with explicit damping elements (the mode shapes will not change with other forms of damping, such as modal damping; note that the frequency does not change much unless the modal damping values are very high), then the modal mass will stay unchanged. This could be an argument to prove that the modal mass for a mode of a system with low values of damping stays unchanged from the same mode without damping, which is readily obtainable from a SOL 103 solution. Modal Mass of Modes With Large Values of Damping However, how do we obtain the modal mass from a complex mode if the eigenvector changes considerably from that without explicit element dampers? A pure real mode has all its terms in phase which each other. Different modes will of course be out of phase with each other, but every point in a particular mode will vibrate in phase. And so, for a mode, all points in the structure reach its maximum and minimum at the same phase instant. A complex mode on the other hand will have different points of the structure reaching its maximum at different phase instants, i.e. different points of the structure are out of phase with each other for a particular mode. Of course, different modes are still out of phase with each other. The degree to which these points are out of phase with each other is a measure of the complexity of the mode. An Argand diagram with all the terms of the complex eigenvector plotted will exhibit a narrowband if the mode is only slightly complex. The diagram below shows plots for 4 eigenvector terms. Since there is only a slight phase difference between the terms (angle between the arrows), the 4 terms define an almost real complex eigenvector. Im Re The following eigenvector plot on the other hand is highly complex because of the large phase angle difference between the terms of the eigenvector. Im Re The eigenvectors of cable elements for instance can change considerably when explicit dampers with high coefficients are placed onto them. Then the modal damping values can become very high (such as even 15 to 20% of critical). If this occurs, the real modal mass is a poor representation of the mode. Instead, a complex modal mass must be evaluated. Hence, a real modal approach should thus not be used in this case. Instead a (rather mathematically involved) complex modal forced response analysis is required. Alternatively, a full MDOF analyses should be undertaken to investigate the response. SOL 111 reverts to a direct solution technique (akin to SOL 108) when there is either viscous or structural element damping as the equations of motion cannot be orthogonalized. But the unknowns are still the modal responses and not the physical responses. And because with damping the modes are really complex modes, there is greater difficulty in capturing all the response using the real modes. Hence, even more modes are thus required to capture the response accurately in SOL 111 with element damping. Thus if elemental damping is high, the direct method SOL 108 may be more appropriate. 339 Structural Engineering Analysis and Design Second Edition 4.3.6 MSC.NASTRAN Decks 4.3.6.1 GL, ML Modal Forced Frequency Response Analysis $ EXECUTIVE CONTROL SECTION SOL 111 $ CASE CONTROL SECTION $ Sets defining grid ids or element ids SET < Number > = 1 THRU 100, 211, 343, < etc > $ Grid output of displacement, velocity and acceleration for excitation frequencies $ SORT1 lists the results by frequency whilst SORT2 lists the results by grid id DISPLACEMENT(,,) = ALL/ VELOCITY(,,) = ALL/ ACCELERATION(,,) = ALL/ $ Grid output of applied load vector OLOAD(,,) = ALL/ $ Grid output of modal responses (in modal space) SDISPLACEMENT(,,) = ALL/< Mode Number > SVELOCITY(,,) = ALL/< Mode Number > SACCELERATION(,,) = ALL/< Mode Number > $ Grid output of real eigenvector for the a-set SVECTOR() = ALL/ $ Grid output of SPC forces SPCFORCES(,,) = ALL/ $ Element output of force, stress and strain ELFORCE(,,) = ALL/ ELSTRESS(,,) = ALL/ STRAIN(,,) = ALL/ $ Analysis Cards SPC = < ID of SPC Cards Defined in Bulk Data > METHOD = < ID IN EIGRL > FREQUENCY = < ID OF FREQi > $ XY plot output OUTPUT(XYPLOT) XYPUNCH RESPONSE /() XYPUNCH RESPONSE /() XYPUNCH RESPONSE /() $ BULK DATA EIGRL ID Lower Frequency (Hz) Upper Frequency (Hz) FREQ1 ID fstart ∆f FREQ4 ID flower fupper bound bound Number of Eigenvalues Eigenvalue Normalization Method Number of ∆f FSPD NFM All FREQi entries with the same selected ID, selected by the FREQUENCY entry in the Case Control Section, will be combined. The FREQ1 bulk data entry selects the frequencies at which the frequency response analysis is performed. It is important to specify a fine enough frequency step size ∆f to adequately predict peak response. Use at least five to ten points across the half-power bandwidth. For maximum efficiency, an uneven frequency step size should be used. Smaller frequency spacing should be used in regions near resonant frequencies, and larger frequency step sizes should be used in regions away from resonant frequencies. FREQ4 defines a frequency spread FSPD for each and every normal mode that occurs within the bounds of the frequency range with NFM evenly 340 Structural Engineering Analysis and Design Second Edition spaced frequencies per spread. Hence, to choose 11 equally spaced frequencies across a frequency band of 0.7fn to 1.3fn for each natural frequency within flower bound and fupper bound, FSPD = 0.30 and NFM = 11. The spread should definitely be greater than the half-power bandwidth, which for a SDOF system is approximately 2ζfn because ζ ≈ (f2-f1)/2fn hence the spread f2-f1 ≈ 2ζfn. FREQ3 specifies excitation frequencies in the range between two modal frequencies. The increments between excitation frequencies are calculated linearly or logarithmically. These frequencies may be clustered towards the end points of the range of towards the center by specifying a cluster parameter. Printed .f06 frequency response output can be in SORT1 or SORT2 format. In the SORT1 format, the results are listed by frequency i.e. for each frequency the results of all grid points are given, whilst in the SORT2 format, the results are listed by grid point i.e. for each grid point the results of all frequencies are given. In the modal frequency response analysis, PARAM, CURVPLOT, 1 and PARAM, DDRMM, -1 are required to obtain SORT1 output. To define frequency frozen structural plots, $ CASE CONTROL SECTION DISPLACEMENT(PLOT,PHASE)=ALL $ BULK DATA PARAM,DDRMM,-1 PARAM,CURVPLOT,1 For each frequency of excitation, the magnitude of the response at each and every point in the structure is animated with the phase information. It is meaningless and impossible to plot the real and imaginary components, as the animation requires the phase difference between different points in the structure. It is prudent to limit the frequencies of excitation so as to limit the amount of output. 341 Structural Engineering Analysis and Design Second Edition 4.3.6.1.1 Applied Load Excitations Applied load excitations are as described in direct forced frequency response analysis. 4.3.6.1.2 Enforced Motion Enforced motion is as described in direct forced frequency response analysis. 4.3.6.1.3 Damping Viscous and structural modal damping is defined as follows. TYPE refers to the type of damping units, i.e. whether structural damping G (default), critical damping CRIT or quality factor Q. The values of fi and gi define pairs of frequencies and damping. Straight-line interpolation is used for modal frequencies between consecutive fi values. Linear extrapolation is used for modal frequencies outside the entered range. ENDT ends the table input. If PARAM, KDAMP, 1 then the modal damping is processed as critical damping and if PARAM, KDAMP, -1 then the modal damping is processed as structural damping, NASTRAN internally making use of ζi = Gi/2 and Qi = 1/Gi to convert to the required coefficient from that specified by TYPE. $ CASE CONTROL SECTION SDAMPING = < ID IN TABDMP1 > $ BULK DATA PARAM, KDAMP, 1 $ modal damping processed as critical damping PARAM, KDAMP, -1 $ modal damping processed as structural damping, complex stiffness TABDMP1 ID TYPE f1 g1 f2 g2 F3 g3 f4 f5 g5 f6 g6 … … ENDT 342 g4 Structural Engineering Analysis and Design Second Edition 4.3.6.2 GL, ML P-∆ (KGA From KEA) Modal Forced Frequency Response Analysis It is often necessary to incorporate the reduction in bending stiffness of gravity load resisting columns for the analysis of lateral loads. The following procedure is undertaken. Phase 1 Perform static analysis (with loads that cause the greatest negative or positive geometric stiffness) based on [KEA] but include the segyroa.v2001 alter prior to the Case Control Section in order to compute the geometric stiffness matrix [KGA]1 (and output into a .pch file) based on the generated element loads from the [KEA] static analysis. Phase 2 A SOL 111 is undertaken based on [KEA] + [KGA]1 with the k2gg=ktjj statement in the Case Control Section and the outputted .pch file which contains the ktjj matrix in the Bulk Data. The responses at this stage represent the P-∆ (KGA From KEA) response to the dynamic excitation. The following equivalent alternative procedure can also be employed. $ CASE CONTROL SECTION SUBCASE 1 LABEL = Static Preload Load Case LOAD = < ID of FORCEi, MOMENTi, PLOADi, GRAV, LOAD, SPCD Cards in Bulk Data > TEMP(LOAD) = < ID of TEMP, TEMPRB, TEMPP1 Cards in Bulk Data > DEFORM = < ID of DEFORM Cards in Bulk Data > SUBCASE 2 LABEL = P-∆ Modal Frequency Response Analysis STATSUB(PRELOAD) = 1 DLOAD = < ID OF RLOAD1 or RLOAD2 > The method is valid when only the prestress is judged to affect the geometric stiffness such as in the compressive preload of building columns due to gravitational loads and the prestressing of extremely taut cables that sag very little under gravity but not in systems such as suspension bridges. Where lateral loads are large enough to affect the geometry of the system with prestress, then a repetitive P-∆, SOL 106, implicit dynamic relaxation SOL 129 or explicit dynamic relaxation must be employed. But in single P-∆ analysis, because cables do not have much elastic bending stiffness, the initial static preload subcase should only include the prestress and not gravity as including gravity is the same as solving two linear static problems of stiffness KEA with preload and gravity as the applied loads respectively. Clearly, in the gravity case, it is nonsensical as the cables do in reality have differential stiffness (from the prestress) to resist the gravitational force. Prestress in one direction (i.e. along the axis of cable) will cause a differential stiffness in the orthogonal direction. Gravity acts in the orthogonal direction and hence cannot be accounted for in the calculation of the prestress in this single P-∆ analysis. To quantitatively decide if gravity need not be considered in contributing to the differential stiffness of the cables, a static P-∆ analysis should be carried out, the first subcase being a SOL 101 with only the prestress as applied loads and the second subcase a P-∆ SOL 101 (i.e. utilizing the induced prestress from the first subcase to form a geometric stiffness matrix) with both the gravity and prestress included as applied loads. If the difference in the cable element forces between subcases 1 and 2 is negligible, then gravity has little influence in affecting the geometric stiffness. If there is a major difference in the cable element force, then clearly, gravity will affect the geometric stiffness and as such, a repetitive P-∆ , SOL 106, implicit dynamic relaxation or explicit dynamic relaxation must be used to converge to the true KT. Likewise, in the single P-∆ analysis of multi-storey buildings, gravity (and only gravity) acts in axis of columns to generate prestress, and the differential stiffness is computed for the orthogonal direction reducing resistance to lateral wind forces, applied in the second subcase with gravity too. 343 Structural Engineering Analysis and Design Second Edition When a static subcase is specified for linear transient response analysis (SOLs 109 and 112) with STATSUB(PRELOAD), the data recovery is controlled by PARAM, ADSTAT. By default (YES) the static solution will be superimposed on the dynamic response solution (displacement, stress and SPCForce). The relative solution can be obtained in reference to the static solution point by PARAM, ADSTAT, NO. No provision is made for frequency response analysis, because the static responses contribute only to the zero frequency response. The STATSUB(PRELOAD) computes the differential stiffness due to the prestress and also the follower force. The follower force is calculated and incorporated by the use of PARAM, FOLLOWK, YES. We know how the prestress affects the differential stiffness, namely a tensile prestress causing an increase in stiffness. The effect of the follower force on the stiffness is different. For example, for a cylinder under external pressure critical buckling load may be overestimated (even though the mode shapes are similar) in a SOL 105 and the natural frequencies in vibration may be underestimated (even though the mode shapes are similar) in a SOL 103 in the absence of follower stiffness. To the contrary, these observations are reversed in case of centrifugal loads. Centrifugal forces as a constant (static) load are applied by a Bulk Data RFORCE to any elements that have masses. The follower stiffness due to centrifugal load has the effect of lowering stiffness (although the centrifugal load tensioning effect increases stiffness), consequently lowering natural frequencies (even though the mode shapes are similar) in a SOL 103 and lowering the buckling loads (even though the mode shapes are similar) in a SOL 105. This effect increases as the RPM increases, and it becomes significant when the RPM is over 1000. For moderately geometric nonlinear analysis, exclusion of follower stiffness affects the rate of convergence, but the converged solution is correct. For severely geometric nonlinear analysis, it may not be possible to obtain a converged solution without including follower stiffness. As the geometric nonlinearity intensifies, so is the effect of follower stiffness. Therefore, inclusion of follower stiffness greatly enhances the convergence if the deformation involves severe geometric nonlinearity. 344 Structural Engineering Analysis and Design Second Edition 4.3.6.3 GL, ML P-∆ (KGA From Exact or Approximate KTA) Modal Forced Frequency Response Analysis It is often necessary to include the differential stiffness, especially if there are prestressed cables in the model. To obtain KTA, to be theoretically exact, a GNL SOL 106 (or implicit dynamic relaxation SOL 129 or explicit dynamic relaxation LS-DYNA) with prestress (as temperature loads say) and gravity must be undertaken. Alternatively, an approximation to KTA can be obtained by repetitive P-∆ static analyses with the prestress (as temperature loads say) and gravity applied. The procedure to obtain this approximate KTA will be presented. Note that the approximate KTA will be the summation of the elastic stiffness KE at the undeflected (by the prestress and gravity) state but KG at the deflected (by the prestress and gravity) state. Hence if KE changes considerably during the application of the prestress, a full SOL 106 (or implicit dynamic relaxation SOL 129 or explicit dynamic relaxation LS-DYNA), which converges to the KE and KG at the deflected (by the prestress and gravity) state should be employed. Hence for the modelling of a suspension bridge where there is a great change in geometry (known in the bridge industry as form-finding, so-called because it is necessary to find the form or shape of the catenary suspension cables), it may be prudent to employ SOL 106 (or implicit dynamic relaxation SOL 129 or explicit dynamic relaxation LSDYNA), but for a high tension low sag cable on say a tower with prestressed cables, the repetitive P-∆ static analysis may be adequate. The repetitive P-∆ analysis basically involves a number of iterations of linear static analyses to obtain an approximate KTA. Note again that A refers to the initial undeflected (by the collapsing load) state, but deflected by the prestress and gravity. To perform the repetitive P-∆ analysis, a static analysis is performed based on KEA with temperature loads and gravity to generate forces in the structural elements, which in turn provides input for the computation of KGiAKTm where m is the iterations. Repetitive static analysis is performed with the prestress and gravity updating the stiffness matrix KEA + KGiAKTm-1 + KGiAKTm until convergence of displacements is obtained. The tangent stiffness at this stage is the approximate converged tangent stiffness matrix KTA = KEA + KGiAKT. The converged displacements represent the approximate P-∆ (KGA From Approximate KTA) static response to the initial prestress loads. The converged geometric stiffness at this stage would be that based upon the approximate tangent stiffness matrix KTA, i.e. KGiAKT. Phase 1 Perform static analysis (with prestress and gravity) based on [KEA] but include the segyroa.v2001 alter prior to the Case Control Section in order to compute the geometric stiffness matrix [KGA]1 (and output into a .pch file) based on the generated element loads from the [KEA] static analysis. Phase 2 Perform static analysis (with prestress and gravity) based on [KEA] + [KGA]1 by including the k2gg = ktjj statement in the Case Control Section, the outputted .pch file which contains the ktjj matrix in the Bulk Data and the segyroa.v2001 alter prior to the Case Control Section to compute the [KGA]2 (and output into the .pch file overwriting previous data) based on the generated element loads from the [KEA] + [KGA]1 static analysis. Phase 3 Repeatedly perform the Phase 2 static analysis (with prestress and gravity) based on [KEA] + [KGA]i for i = 2 to n where n represents the number of iterations required for the change in deflections between analyses to become negligible. This would signify that the change in the [KGA] matrix become negligible and the correct [KGA] is attained. The deflections and the other responses at this stage represent the P-∆ (KGA From Approximate KTA) static response to the prestress and gravity. The stiffness of the structure is KTA. Phase 4 A SOL 111 is undertaken with the k2gg=ktjj statement in the Case Control Section and the outputted .pch file which contains the latest ktjj matrix in the Bulk Data. The responses at this stage represent the P-∆ (KGA From Approximate KTA) response to the dynamic excitation. 345 Structural Engineering Analysis and Design Second Edition 4.3.7 4.3.7.1 Hand Methods Verification Determination of Maximum Dynamic Displacement for Deterministic Frequency Domain Loading by Transforming the Coupled MDOF Linear Damped ODEs To a Set of Independent (Uncoupled) SDOF ODEs and Solving the Independent Equations in a Manner Similar to Solving a SDOF ODE Linear frequency domain hand methods are capable of analyzing: - Multi-Modal Response To Deterministic Periodic Harmonic Long Duration Loading Functions A coupled MDOF system of linear ODEs must be uncoupled to a set of independent SDOF system of linear ODEs if any feasible hand method computation is to be employed. These independent SDOF ODEs can be solved using standard techniques of solving SDOF linear dynamic ODEs. The final stage to the analysis is to employ a modal superposition method to express the total response as a summation of the results from the solution of the individual modal equations. Note that since the modal frequencies and the corresponding mode shapes are required to uncouple the coupled MDOF ODEs, the real eigenvalue analysis must be performed first. It was shown that a system of coupled MDOF ODEs could be reduced to a system of independent SDOF ODEs by employing the orthogonality properties of real modes −ω 2 M i ξ i (ω) + iC i ωξ i (ω) + K i ξ i (ω) = Pi (ω) where the generalized (or modal) terms are obtained from solving the real eigenvalue problem M i = {φ i } [M ]{φ i } T C i = {φ i }T [C]{φ i } = ζ i 2M i ω n i K i = {φ i } [K ]{φ i } = ω 2ni M i T Pi (ω) = {φ i } {P(ω)} T The modal properties (i.e. modal masses, modal frequencies and hence modal stiffness) can be obtained by performing a real modal analysis SOL 103 and if required the modal damping can also be incorporated from a complex modal analysis SOL 107. The normalization of the mode shapes can be arbitrary. The normalization technique employed will not affect the value of the modal frequencies but of course will determine the values of the modal masses (and hence modal damping and stiffnesses) and the (amplitude of the) modal force. Although the normalization technique is arbitrary, it is recommended that the normalization employed would facilitate the calculation of the (amplitude of the) modal force since this is a hand calculation. To facilitate the computation, it is wise to choose the normalization to be unity at the DOF of application of the external excitation. Either way, the modal force (for a particular mode) for discrete loading points is calculated as follows Pi (ω) = {φ i } {P(ω)} T Had the loading been continuous, a continuous modal force can also be calculated by hand (or a spreadsheet) as follows L Pi (ω) = ∫ φ i ( x ){P( x , ω)}dx 0 For the special case, which is most common in reality, when the complex harmonic force vector is independent of the frequency of excitation and simply real, we have {P(ω)} = {p0} and hence, [ ] = Re al [{p }e ] {P( t )} = Re al {P(ω)}e iωt iωt 0 hence Pi (ω) = {φ i } {p 0 } T = p 0i 346 Structural Engineering Analysis and Design Second Edition There will be n uncoupled ODEs for n natural modes. These are now simply SDOF ODEs, which can be solved using complex arithmetic. Hence, the complex modal response (in modal space) ξ i (ω) = Pi (ω) p 0i = 2 − ω M i + iC i ω + K i − ω M i + i C i ω + K i 2 From complex number the ory x + iy =  x 2 + y 2 e iθ , θ = tan −1 ( y / x )   Changing the denominato r to a polar complex form p 0i Ci ω 2ζ i ω / ω ni ξ i (ω) = , θ i = tan −1 = tan −1 2 2 2 K i − Miω 1 − ω 2 / ω ni K i − M i ω 2 + (C i ω)2 e iθi ( ξ i (ω) = ( ) (1 − ω p 0i / K i 2 / ω ni ) 2 2 + (2ζ i ω / ω ni )2 e −iθi , θ i = tan −1 2ζ i ω / ω ni (1 − ω 2 / ω ni 2 ) This can be written very illustratively as ξ i ( ω) = D i ( ω) p 0i − iθi 2ζ i ω / ω ni e , θ i = tan −1 2 Ki 1 − ω 2 / ω ni ( ) where the real modal amplificat ion factor and its maximum are 1 1 D i (ω) = ; D i max = 2 2 2 2ζ 1 − ζ 2 1 − ω 2 / ω ni + (2ζ i ω / ω ni ) ( ( ) Thus, the steady-state solution in the time domain {u (t )} = Re al [[Φ ]{ξ(ω)}e iωt ]   {u (t )} = Re al [Φ ]D(ω) p 0 e −iθ e iωt    K   {u (t )} = Re al [Φ ]D(ω) p 0 e i( ωt -θ)  K    {u (t )} = [Φ ]D(ω) p 0 cos(ωt - θ)  K  Note that this expression is to be interpreted as {u (t )} = [{φ}1 ... {φ}i p 01   cos(ωt - θ1 )   D1 (ω) K1   ...   p 0i   ... {φ}n ] D i (ω) cos(ωt - θi )  Ki   ...   p 0n   cos(ωt - θ n ) D n (ω) K n   347 ) ) Structural Engineering Analysis and Design Second Edition Note that p0i corresponds to the amplitude of the modal loading function Pi(ω) and not simply the amplitude of the loading function {P(ω)}, i.e. p0 at any particular node. Of course, if the normalization of the mode was such that it was unity at the DOF of application of the external force with amplitude p0 then, p0i will be equal to p0. For a 2 DOF system, this expression would be  u 1 ( t )   φ11  = u 2 ( t ) φ 21 p0   D1 (ω) 1 cos(ωt - θ1 )   φ12   K1     p φ 22   0 D 2 (ω) 2 cos(ωt - θ 2 )   K2 The above computation takes into account the phase difference between the responses of different modes. It is important to point out that the maximum of the modal responses ξi(ω) do not occur at the same time. The frequency domain response ODE can only be solved for a particular excitation frequency ω at a time. For a particular ω there will be different responses ξi(ω) from different modes, differing in amplitude of response Di(ω), static displacement and in phase θi. Because there is a difference in phase angle between the responses of each and every mode from θ i = tan −1 2ζ i ω / ωni (1 − ω 2 / ωni 2 ) the exact solution involves maximizing a complicated trigonometric expression with many phase angles. The exact solution can be obtained by expanding the general u(t) expression to include all the modes considered, and only then maximised. However, this may prove to be mathematically involved if differentiation is to be performed analytically by hand (the computerized method of course performs the response calculation at discrete frequency points as it is not just the maximum that is of interest). An alternative would be to instead of maximising the physical response, maximise the modal responses and then only superpose the modal responses for the physical response. 1 D i max = 2ζ 1 − ζ 2 ( ξ i max = D i max (ω) ) p 0i Ki This is equivalent to the response spectrum method (only that the procedure is employed on a deterministic loading function instead of a random function). The square root of sum of squares (SRSS) of the maximum modal contributions as follows, depicted for a 2 DOF dynamic system.  u 1 max   (φ11ξ1 max )2 + (φ12 ξ 2 max )2   =  u 2 max   (φ 21ξ1 max )2 + (φ 22 ξ 2 max )2  Alternatively, the Complete Quadratic Combination (CQC) method is used if the modal natural frequencies are too close to each other (within about 10 %). This is based on random vibration theory. Of course, the upper limit combination would be to choose all the eigenvectors to have the maximum modal response at the same time. Often, we need to ascertain other types of response such as velocity and acceleration. We know that,  {u ( t )} = Re al [Φ ]D(ω)   p 0 i ( ωt -θ)  e  K  348 Structural Engineering Analysis and Design Second Edition Hence the velocity, {u&(t )} = Re al [Φ]iωD(ω) p0 e i (ωt-θ)  K    {u&(t )} = −ω[Φ ]D(ω) p0 sin(ωt - θ) K   And the acceleration,   p  u&( t )} = Re al [Φ ]− ω2 D(ω) 0 e i ( ωt -θ)  {&    K p   u&( t )} = −ω2 [Φ ]D(ω) 0 cos(ωt - θ)  {&  K  The differentiation of the complex vector representing the displacement is equivalent to multiplying the length of the vector by ω and turning it ahead by 90 degrees. Multiplying any complex number by imaginary i is equivalent to a rotation of 90 degrees. Hence the velocity leads the displacement by 90 degrees and the acceleration leads the velocity by 90 degrees. The magnitude of the velocity is ω times that of the displacement and the magnitude of the acceleration is ω times that of the velocity. In all cases, it is implicitly understood that it is the real part of the complex number that represents the physical harmonic motion. Note that the total response is obtained by multiplying the eigenvectors by their corresponding modal amplitude factor, which is an indication of the prominence of the mode in the response. It is often the case that lower modes of vibration will have greater prominence. Hence, only a few of the initial prominent modes need to be evaluated in the expression. However, an important point to observe is that since the velocity and acceleration total responses in the time domain are a function of the frequencies and the square of the frequencies respectively on top of the usual modal amplitude factors, this would mean that the prominence of higher modes become more significant when velocities and accelerations are computed. Ideally, the responses in the time domain should be maximised to obtain the maximum response. But if this proves to be difficult, the modal responses can be maximised and combined using some superposition method such as SRSS or CQC (effectively a response spectrum analysis on a deterministic loading function). For whatever response be it the displacement, velocity acceleration or force, the individual modal responses should first be calculated in terms of time t, then maximised, then only combined for the physical response with some method of superposition. Do not maximise the modal displacement response and base the other velocity and acceleration responses on that. 349 Structural Engineering Analysis and Design Second Edition A forced response analysis of a shear frame (be it to model a building or water tank) is illustrated in MAPLE 7. All units in SI. M u1 10000cos4.5826t EI = 560000000 M = 400000 L=4 EI 2L M M u2 EI 2L L EI System and Frequency Domain Excitation Description - User Input > restart; with(LinearAlgebra): DOF:=2: EI:=560000000: M:=400000: L:=4: MASS:=Matrix([[M,0],[0,2*M]]); KE:=Matrix([[3*EI/L^3,-3*EI/L^3],[-3*EI/L^3,9*EI/L^3]]); MODALDAMPING:=Matrix([[0.01,0],[0,0.01]]); # Excitation - P(w) is the magnitude of the excitation, i.e. P(t)=Re[P(w)EXP(iwt)] w:=4.5826: P(w):=Matrix([[10000],[0]]); 0 400000 MASS :=    0 800000   26250000 -26250000 KE :=  -26250000 78750000   .01 MODALDAMPING :=  0  0  .01 10000 P( 4.5826 ) :=    0  Modal Properties of System - Solution of Real Eigenvalue Problem [K-λM]{φ}={0} - Note that Eigensolution may not arrange the roots sequentially - MAX normalization of the Eigenvectors > Eigensolution:=Eigenvectors(MatrixInverse(MASS).KE): lambda:=Matrix(Eigensolution[1],shape=diagonal): wn:=map(sqrt,evalf(lambda)); Phi:=Eigensolution[2]; for j from 1 to DOF do eig:=0: for i from 1 to DOF do eig:=eig,Phi[i,j]; end do; for i from 1 to DOF do Phi[i,j]:=Phi[i,j]/max(eig); end do; end do: Phi:=Phi; 350 Structural Engineering Analysis and Design Second Edition 0.  5.728219619 wn :=    0. 11.45643924   2 -1 Φ :=   1 1   1  Φ :=  1  2 -1   1  Uncoupling The Equations of Motion > MODALMASS:=evalf(Transpose(Phi).MASS.Phi); MODALSTIFFNESS:=evalf(Transpose(Phi).KE.Phi); MODALFORCE:=evalf(Transpose(Phi).P(w)); 0. 600000.   MODALMASS :=  7  0. .1200000 10   .19687500 10 MODALSTIFFNESS :=  0.  8 0.   .157500000 109  10000.  MODALFORCE :=  -10000.   Modal Responses Re[ξi] = Di(w)Poi/Ki cos(wt-θi) > D(w):=Vector(DOF): for i from 1 to DOF do D(w)[i]:=1/((1-w^2/lambda[i,i])^2+(2*MODALDAMPING[i,i]*w/lambda[i,i]^(1/2))^2)^(1/2); end do; xi:=Vector(DOF): for i from 1 to DOF do xi[i]:=D(w)[i]*MODALFORCE[i,1]/MODALSTIFFNESS[i,i]*cos(w*tarctan(2*MODALDAMPING[i,i]*w/lambda[i,i]^(1/2)/(1-w^2/lambda[i,i]))); end do: xi:=evalf(xi); D( 4.5826 ) := 2.775090553 1 D( 4.5826 ) := 1.190424609 2  .001409569805 cos ( 4.5826 t − .04441628701)  ξ :=  −.00007558251486cos ( 4.5826 t − .009523591344)   Physical Response in Time Domain > u(t):=Vector(DOF): u(t):=Phi.xi;  .001409569805 cos ( 4.5826 t − .04441628701) + .00007558251486cos ( 4.5826 t − .009523591344)  u( t ) :=  .0007047849025cos ( 4.5826 t − .04441628701) − .00007558251486cos ( 4.5826 t − .009523591344)   Plot of Response in Time Domain > variablelegend:=seq(convert(u[i],string),i=1..DOF): plot([seq(u(t)[i],i=1..DOF)], t=0..10, Displacement,title="Steady-State Displacement Response", legend=[variablelegend]); 351 Structural Engineering Analysis and Design Second Edition An absolutely equivalent method of solving the equations in the frequency domain is to work in real and imaginary terms instead of in terms of magnitude and phase. As before, the complex modal response (in modal space) is ξ i (ω) = p 0i − ω M i + iC i ω + K i = p 0i − ω M i + K i + iC i ω = (1 − ω 2 2 p 0i / K i 2 ) / ω ni + i(2ζ i ω / ω ni ) 2 Instead of the polar form, this can be written in terms of the real and imaginary parts ( ) 2  p 0i  (2ζ i ω / ω ni ) 1 − ω 2 / ω ni   −i 2 2 2 2  2 K i  1 − ω 2 / ω 2 + (2ζ ω / ω )2 1 − ω / ω + 2 ζ ω / ω ( ) ni i ni ni i ni   ξ i (ω) = ξ iREAL (ω) − iξ iIMAG (ω) ξ i (ω) = ( ) ( ) Thus, the steady-state solution in the time domain {u ( t )} = Re al [[Φ ]{ξ REAL (ω) − iξ IMAG (ω)}e iωt ] {u ( t )} = Re al [[Φ ]{ξ REAL (ω) − iξ IMAG (ω)}(cosωt + isinωt )] {u ( t )} = [Φ ]{{ξ REAL (ω)}cos ωt + {ξ IMAG (ω)}sin ωt} Note that this expression is to be interpreted as {u ( t )} = [{φ}1 ... {φ}i where D iREAL (ω) = D iIMAG (ω) =  p 01   K (D1REAL (ω) cos ωt + D1IMAG (ω) sin ωt )   1  ...   p  ... {φ}n ] 0i (D iREAL (ω) cos ωt + D iIMAG (ω) sin ωt )  K  i  ...    p 0n (D  ) ( ω ) cos ω t + D ( ω ) sin ω t nREAL nIMAG K   n  (1 − ω / ω ) / ω ) + (2ζ ω / ω 2 2 (1 − ω ni 2 2 2 ni i ni )2 (2ζ i ω / ω ni ) (1 − ω2 / ωni 2 )2 + (2ζ i ω / ωni )2 This method is very useful because the final expression being in cos and sin means that we can very quickly find the maximum response (i.e. the steady-state response) as MAX (Acosωt + Bsinωt) = (A2+B2)½. At a particular DOF j, the steady state response will then be Steady − State Response, u jMAX  =   n ∑ i 2   p 0i φ ij D iREAL (ω)  +  Ki   n ∑ i  p 0i φ ij D iIMAG (ω)  Ki  2 This procedure is now implemented in the above MAPLE example, showing identical results in the end. 352 Structural Engineering Analysis and Design Second Edition System and Frequency Domain Excitation Description - User Input > restart; with(LinearAlgebra): DOF:=2: EI:=560000000: M:=400000: L:=4: MASS:=Matrix([[M,0],[0,2*M]]); KE:=Matrix([[3*EI/L^3,-3*EI/L^3],[-3*EI/L^3,9*EI/L^3]]); MODALDAMPING:=Matrix([[0.01,0],[0,0.01]]); # Excitation - P(w) is the magnitude of the excitation, i.e. P(t)=Re[P(w)EXP(iwt)] w:=4.5826: P(w):=Matrix([[10000],[0]]); 0 400000 MASS :=    0 800000    26250000 -26250000 KE :=  -26250000 78750000   .01 0  MODALDAMPING :=   0 .01   10000 P( 4.5826 ) :=    0  Modal Properties of System - Solution of Real Eigenvalue Problem [K-λM]{φ}={0} - Note that Eigensolution may not arrange the roots sequentially - MAX normalization of the Eigenvectors > Eigensolution:=Eigenvectors(MatrixInverse(MASS).KE): lambda:=Matrix(Eigensolution[1],shape=diagonal): wn:=map(sqrt,evalf(lambda)); Phi:=Eigensolution[2]; for j from 1 to DOF do eig:=0: for i from 1 to DOF do eig:=eig,Phi[i,j]; end do; for i from 1 to DOF do Phi[i,j]:=Phi[i,j]/max(eig); end do; end do: Phi:=Phi; 0. 5.728219619  wn :=    0. 11.45643924   2 Φ :=  1  1  Φ :=  1  2 -1  1 -1   1  Uncoupling The Equations of Motion > MODALMASS:=evalf(Transpose(Phi).MASS.Phi); MODALSTIFFNESS:=evalf(Transpose(Phi).KE.Phi); MODALFORCE:=evalf(Transpose(Phi).P(w)); 0. 600000.   MODALMASS :=   0. .1200000 107  .19687500 10 MODALSTIFFNESS :=   0.  353 8   .157500000 10  0. 9 Structural Engineering Analysis and Design Second Edition  10000.  MODALFORCE :=  -10000.   Modal Responses Re[ξi] = Poi/Ki { DiREAL(w)cos(wt)-DiIMAG(w)sin(wt) } > DREAL(w):=Vector(DOF): DIMAG(w):=Vector(DOF): for i from 1 to DOF do DREAL(w)[i]:=(1-w^2/lambda[i,i])/((1w^2/lambda[i,i])^2+(2*MODALDAMPING[i,i]*w/lambda[i,i]^(1/2))^2); DIMAG(w)[i]:=(2*MODALDAMPING[i,i]*w/lambda[i,i]^(1/2))/((1w^2/lambda[i,i])^2+(2*MODALDAMPING[i,i]*w/lambda[i,i]^(1/2))^2); end do; xi:=Vector(DOF): for i from 1 to DOF do xi[i]:=MODALFORCE[i,1]/MODALSTIFFNESS[i,i]*(DREAL(w)[i]*cos(w*t)+DIMAG(w)[i]*sin(w*t)); end do: xi:=evalf(xi); DREAL( 4.5826 ) := 2.772353645 1 DIMAG( 4.5826 ) := .001344426180 525 1 16 DREAL( 4.5826 ) := 1.190370624 2 DIMAG( 4.5826 ) := .0002473924464 525 2 4  .001408179629 cos ( 4.5826 t ) + .00006258727349sin( 4.5826 t )   ξ :=  −.00007557908724cos ( 4.5826 t ) − .719806102510-6 sin( 4.5826 t )   Physical Response in Time Domain > u(t):=Vector(DOF): u(t):=Phi.xi;  .001483758716 cos ( 4.5826 t ) + .00006330707959sin( 4.5826 t )  u( t ) :=  .0006285107273cos ( 4.5826 t ) + .00003057383064sin( 4.5826 t )   Plot of Response in Time Domain > variablelegend:=seq(convert(u[i],string),i=1..DOF): plot([seq(u(t)[i],i=1..DOF)], t=0..10, Displacement,title="Steady-State Displacement Response", legend=[variablelegend]); 354 Structural Engineering Analysis and Design Second Edition 4.4 4.4.1 GL, ML Implicit (Complex) Modal Frequency Response Analysis Mathematical Formulation of Analysis SOL 111 performs a modal forced frequency response analysis. It utilizes the real modal properties to decouple the equations of motion when there is no elemental structural and/or viscous damping within the system. With the existence of elemental structural and/or viscous, the real modal properties cannot decouple the couple ODEs. In this case, SOL 111 then performs the forced frequency response analysis using a direct approach on the coupled ODEs, but in the modal coordinates instead of the physical coordinates. With sufficient modes (sufficient modal variables), a SOL 111 solution will yield the same answer as a SOL 108 solution. However, the use of the FREQ4 card, which bases the excitation frequencies to be solved for on the real natural frequencies may prove to be insufficient. This is because with high values of elemental viscous damping, certain local modes can be totally eliminated. For instance, viscous dampers with high coefficients of damping on cables can considerably alter the natural frequency of the local mode and even eliminate a local mode altogether. In this case, the FREQ4 card will not capture the response at the damped natural frequency. Hence, these damped natural frequencies need to be known (by performing a SOL 107) before choosing the excitation frequencies to be solved for using FREQ2 cards. If however, a modal approach is still intended with the existence of structural and/or viscous damping, the complex modal properties must be employed. It is thus necessary to find new orthogonality properties of modes (complex modes now) in order to be able to diagonalize the matrices. The response analysis is called the complex modal forced response analysis. The mathematical formulation of the solution scheme is quite involved. In principle, in order to employ a modal approach, we need to reduce a set of coupled ODEs to a set of uncoupled ODEs that can be solved independently of each other. In order to do that, we need to establish orthogonality conditions. A similar procedure employed for establishing real modal orthogonality conditions can again be utilized to determine the complex modal orthogonality conditions. The decision of whether such an involved process is required lies with the degree of complexity of the modes. If the modes are only slightly complex, then a real modal approach might well be justified. In order to ascertain the level of complexity of a particular mode, each term within the complex eigenvector is plotted on an Argand diagram i.e. the imaginary component versus the real component. An almost real mode shape does not necessarily have vector terms near 0 or 180 degrees. What matters is the relative phase between different terms. A pure real mode has all its terms in phase which each other. Different modes will of course be out of phase with each other, but every point in a particular mode will vibrate in phase. And so, for a mode, all points in the structure reach its maximum and minimum at the same phase instant. A complex mode on the other hand will have different points of the structure reaching its maximum at different phase instants, i.e. different points of the structure are out of phase with each other for a particular mode. Of course, different modes are still out of phase with each other. The degree to which these points are out of phase with each other is a measure of the complexity of the mode. An Argand diagram with all the terms of the complex eigenvector plotted will exhibit a narrowband if the mode is only slightly complex. The diagram below shows plots for 4 eigenvector terms. Since there is only a slight phase difference between the terms (angle between the arrows), the 4 terms define an almost real complex eigenvector. Im Re 355 Structural Engineering Analysis and Design Second Edition The following eigenvector plot on the other hand is highly complex because of the large phase angle difference between the terms of the eigenvector and as such a complex modal approach needs to be undertaken if a modal approach is intended at all. A direct approach is most recommended to avoid the mathematical complexities. Im Re The modal approach in the frequency domain based on real modal properties is first described. This is the approach used by SOL 111 only when there is no elemental structural or elemental viscous damping. The coupled system of ODEs of the undamped forced vibration equation of motion is [M ]{& u&( t )} + [K ]{u ( t )} = {P( t )} To solve the equation in the frequency domain, we let {u ( t )} = Re al [[Φ ]{ξ(ω)}e iωt ] Hence −[M ][Φ ]{ξ(ω)}ω 2 e iωt + [K ][Φ ]{ξ(ω)}e iωt = {P(ω)}e iωt −ω 2 [M ][Φ ]{ξ(ω)} + [K ][Φ ]{ξ(ω)} = {P(ω)} It can be shown that the orthogonality condition of the normal modes is {φ i }T [[M ] + [K ]]{φ j }= 0 if i≠ j T Hence, premultiplying by [Φ ] reduces the coupled system of ODEs to a system of uncoupled ODEs T T T −ω 2 [Φ ] [M ][Φ ]{ξ(ω)} + [Φ ] [K ][Φ ]{ξ(ω)} = [Φ ] {P(ω)} −ω 2 [M]{ξ(ω)} + [K ]{ξ(ω)} = {P(ω)} The matrices [M] and [K] are thus diagonal. The modal approach in the frequency domain based on complex modal properties is now described. Complex eigenvalue analysis with viscous (and structural optional) damping, for each mode i, NASTRAN outputs, two complex roots which are a complex conjugate pair, α i + iωdi and α i − iωdi , where α i is negative and represents the decaying constant ωdi is positive and represents the damped natural circular frequency two complex eigenvectors which are a complex conjugate pair, {φ R + iφ I }i and {φ R − iφ I }i Complex eigenvalue analysis with only structural (and no viscous) damping, for each mode i, NASTRAN outputs, one complex root, α i + iωdi , where α i is negative and represents the decaying constant ωdi is positive and represents the damped natural circular frequency one complex eigenvector, {φ R + iφ I }i 356 Structural Engineering Analysis and Design Second Edition The coupled system of ODEs of the damped forced vibration equation of motion is [M ]{& u&( t )} + [C]{u&( t )} + [K ]{u ( t )} = {P( t )} where [ K ] = (1 + iG )[K ] + i ∑G E [K E ] It can be shown that the orthogonality conditions with viscous (and structural optional) damping are {φ R {φ R [((α + iφ } [((α + iφ I }i )) ] ))[M ] − [K ]]{φ + iω di ) + α j + iω dj [M ] + [C] {φ R + iφ I }j = 0, i + iω di T I ( ) * (α i T j + iω dj R + iφ I }j = 0, and if i≠ j Note that the orthogonality condition with only structural (and no viscous) damping is {φ R + iφ I } T [[M] + [K ]]{φ R + iφ I }j = 0, if i≠ j Clearly, the orthogonality conditions are far more complicated, making the mathematics defining the complex modal forced frequency response analysis very difficult. It will not be attempted here. 357 Structural Engineering Analysis and Design Second Edition 4.5 4.5.1 GL, ML Implicit Direct Frequency Response Analysis Nature of the Dynamic Loading Function The solution method can be used to solve dynamic systems subjected to: (a) Deterministic periodic harmonic long duration loading functions A deterministic periodic forcing function has regularly repeating amplitude. The sine or cosine function is said to be harmonic. Because the periodic function repeats itself, any initial starting transient response is insignificant and the steady state response is of interest, hence the solution is performed in the frequency domain. The starting transient normally decays away after 50-100 cycles of oscillation for light damping. The steady-state oscillatory response occurs at the same frequency as the loading phase shifted due to damping. In this LINEAR FREQUENCY DOMAIN solution, not only that the static response has to be added separately, but also the mean of the dynamic excitation has also got to be added separately as a static response. This is because the mean of the dynamically applied force is not included in the dynamic excitations. Hence the total response in this frequency domain dynamic analysis = static response to mean of dynamic excitation + dynamic response + static response to static loads. 4.5.2 Mathematical Formulation of Analysis This method is not a modal method and so the solution is not a reduced solution and is therefore computationally very expensive as it involves the full mass, stiffness and damping matrices. For small models this type of solution is probably better than a modal frequency response analysis and certainly more accurate. However, for large models it is too inefficient and can only be used to compute response at a handful of frequency locations, where there is doubt in the modal frequency response results. In general, modal frequency response analysis is used when (i) the model is large (ii) many excitation frequencies need to be solved for On the other hand, direct frequency response analysis is employed when (i) the model is small (ii) only a few excitation frequencies need to be solved for (iii) the response due to high frequency excitation is required, as this requires many modes to be computed in the modal frequency response analysis, the computation of the modes being the costly operation in the modal approach (iv) high accuracy is required as the direct approach does not involve mode truncation. The coupled system of ODEs of the undamped harmonically forced vibration equation of motion are given by u&( t )} + [K ]{u ( t )} = {P( t )} [M ]{& In the frequency domain, let {u ( t )} = Re al [{F(ω)}e iωt ] where {F(ω)}is a complex displacement response function vector {P(t )} = Re al [{P(ω)}e iωt ] where {P(ω)}is a complex forcing function vector This transformation is worth a little explanation. The harmonic forcing function in the time domain P(t) is transformed into the frequency domain simply by multiplying {P( t )} = Re al [{P(ω)}e iωt ] {P(ω)} is the complex harmonic forcing function. The harmonic term is eiωt. {P(ω)} can be frequency dependent and/or can even be complex in general. If {P(ω)} is complex, this refers to harmonic loading functions which are out of phase with respect to each other. We usually assume that {P(ω)} is frequency independent and also just real, such that {P(ω)} = {p0}. The frequency domain complex forcing function {P(ω)} is specified in NASTRAN with 358 Structural Engineering Analysis and Design Second Edition the RLOAD1 and RLOAD2 cards. The harmonic term is inferred naturally. It must be stressed that the specified frequency domain excitation is the complex harmonic forcing function {P(ω)} and that the corresponding complex total response vector is {F(ω)}. If {P(ω)} is complex, then {F(ω)} will be complex. If {P(ω)} is only real, then {F(ω)} will be real if there is no damping in the system but will be complex if there is damping in the system. The curves for {F(ω)} versus ω is what is produced by the NASTRAN output in a frequency domain analysis. It can be viewed in its real and imaginary components versus ω, or in its magnitude and phase versus ω, the latter of which is what should be observed to ascertain the response. To summarize Frequency domain loading function from the time domain loading function [ ] {P( t )} = Re al {P(ω)}e iωt where {P(ω)} is the complex loading function vector Frequency domain complex total response function vector is {F(ω)} which is complex in general Time domain total response from the frequency domain complex total response [ {u ( t )} = Re al {F(ω)}e iωt ] Hence on substituti on, −[M ]{F(ω)}ω 2 e iωt + [K ]{F(ω)}e iωt = {P(ω)}e iωt [− ω [M] + [K ]]{F(ω)} = {P(ω)} 2 {F(ω)} = {P(ω)} − ω 2 [M ] + [K ] This equation is solved at each and every specified discrete forcing frequency ω using complex aritmetic. Because the terms are vectors and matrices, there is the requirement for simultaneous equation solvers to ascertain {F(ω)}, this being the reason that the direct approach is far more expensive computationally compared to the modal approach. Finally the total response is {u ( t )} = Re al [{F(ω)}e iωt ] The following damping models are supported by the solution scheme I. elemental damping i. viscous damping Yes ii. structural damping Yes II. modal damping i. viscous damping No ii. structural damping No III. global proportional viscous damping i. mass proportional damping No ii. stiffness proportional damping Yes iii. Rayleigh damping No 359 Structural Engineering Analysis and Design Second Edition With damping, the coupled system of ODEs of the damped harmonically forced vibration equation of motion are given by [M ]{& u&( t )} + [C]{u&( t )} + [K ]{u ( t )} = {P( t )} where [K ] = (1 + iG )[K ] + i [C ] = ∑ [C ∑G E [K E ] E] Hence, −[M ]{F(ω)}ω 2 e iωt + iω[C]{F(ω)}e iωt + [K ]{F(ω)}e iωt = {P(ω)}e iωt [− ω [M] + iω[C] + [K ]]{F(ω)} = {P(ω)} 2 {F(ω)} = −ω 2 {P(ω)} [M] + iω[C] + [K ] This equation is solved at each and every specified discrete forcing frequency ω using complex arithmetic. Unlike the modal frequency response analysis, the direct frequency response analysis requires the solution of simultaneous equations at each forcing frequency, hence explaining its additional cost. Finally the total response is {u ( t )} = Re al [{F(ω)}e iωt ] In direct frequency response analysis, it is not necessary to assume an equivalent viscous form for structural damping as the solution is complex. Hence the element structural damping coefficient Gelement or G parameters do not form a damping matrix [C], instead they form a complex stiffness matrix. The complex response function due to a loading {P(ω)} is defined as {F(ω)} = −ω 2 {P(ω)} [M ] + iω[C] + [K ] The complex transfer function is defined as the complex frequency response function due to unit harmonic excitations [H(ω)] = 1 − ω [M ] + iω[C] + [K ] 2 This is the so-called transfer function that transfers the excitation to the response as follows [ {u ( t )} = Re al [H (ω)]{P(ω)}e iωt ] The (magnitude of the) dynamic amplification function D(ω) is defined as the magnitude of the complex response function {F(ω)} divided by the static displacement. The animation of the forced frequency response is quite indicative of the nature of the response of the structure to harmonic excitations. The forced frequency response analysis will yield for each node, both real and imaginary responses. The animation of the forced response of the structure as a whole (at any particular frequency of excitation) is only of value when we plot the magnitude of the response, and not the individual real or imaginary components. The phase information (which is obtained when the magnitude and argument of the real and imaginary components are obtained) is essential in order to determine the relative phase of the motion of different parts of the structure. Explicit viscous dampers will cause parts of the structure to vibrate clearly out-of-phase. 360 Structural Engineering Analysis and Design Second Edition 4.5.3 MSC.NASTRAN Decks 4.5.3.1 GL, ML Direct Forced Frequency Response Analysis $ EXECUTIVE CONTROL SECTION SOL 108 $ CASE CONTROL SECTION $ Sets defining grid ids or element ids SET < Number > = 1 THRU 100, 211, 343, < etc > $ Grid output of displacement, velocity and acceleration for excitation frequencies $ SORT1 lists the results by frequency whilst SORT2 lists the results by grid id DISPLACEMENT(,,) = ALL/ VELOCITY(,,) = ALL/ ACCELERATION(,,) = ALL/ $ Grid output of applied load vector OLOAD(,,) = ALL/ $ Grid output of d-set displacement, velocity and acceleration SDISPLACEMENT(,,) = ALL/ SVELOCITY(,,) = ALL/ SACCELERATION(,,) = ALL/ $ Grid output of SPC forces SPCFORCES(,,) = ALL/ $ Element output of force, stress and strain ELFORCE(,,) = ALL/ ELSTRESS(,,) = ALL/ STRAIN(,,) = ALL/ $ Analysis Cards SPC = < ID of SPC Cards Defined in Bulk Data > FREQ = < ID OF FREQi > $ XY plot output OUTPUT(XYPLOT) XYPUNCH RESPONSE /() XYPUNCH RESPONSE /() $ BULK DATA FREQ1 ID fstart ∆f Number of ∆f All FREQi entries with the same selected ID, selected by the FREQUENCY entry in the Case Control Section, will be combined. The FREQ1 bulk data entry selects the frequencies at which the frequency response analysis is performed. The FREQ and FREQ2 cards can also be used to define points within the regions of resonance (evaluated by a separate modal analysis prior to the forced response analysis). It is important to specify a fine enough frequency step size ∆f to adequately predict peak response. Use at least five to ten points across the halfpower bandwidth. For maximum efficiency, an uneven frequency step size should be used. Smaller frequency spacing should be used in regions near resonant frequencies, and larger frequency step sizes should be used in regions away from resonant frequencies. Adaptive excitation frequency Bulk Data entries, which depend on the modal frequencies FREQ3, FREQ4 and FREQ5 cannot be used as the modal frequencies are not calculated in the direct response analysis. This is one of the drawbacks of the direct method SOL 108 as opposed to the modal method SOL 112, i.e. it is necessary to spend effort in capturing the peak. SOL 112 does not suffer from this drawback because the solution set is the modal responses and hence the peak is naturally captured. But in SOL 108, it is especially difficult to capture peak when the modal damping is low since the peak is very spiky. Again five to ten points across the half-power bandwidth must be ensured. To check if the peak has been truly captured, a SOL 107 can be used to estimate the modal damping. Then assuming small modal damping the maximum dynamic 361 Structural Engineering Analysis and Design Second Edition amplification would be 1/2ζ. Note that the dynamic amplification curve is obtained from the plotted FRF from NASTRAN by dividing by the static response P/K. It should be okay to use the zero frequency SOL 108 response to estimate the static response P/K, although this assumes that the frequency is close enough to zero and that there is little structural damping in the system. There are of course no modal truncation concerns in this direct approach. The exact estimate of the static response P/K would clearly be to perform a static analysis SOL 101 with a magnitude equal to the amplitude of the frequency domain (sinusoidal) forcing function. Printed .f06 frequency response output can be in SORT1 or SORT2 format. In the SORT1 format, the results are listed by frequency i.e. for each frequency the results of all grid points are given, whilst in the SORT2 format, the results are listed by grid point i.e. for each grid point the results of all frequencies are given. To define frequency frozen structural plots, $ CASE CONTROL SECTION DISPLACEMENT(PLOT,PHASE)=ALL $ BULK DATA PARAM,DDRMM,-1 PARAM,CURVPLOT,1 For each frequency of excitation, the magnitude of the response at each and every point in the structure is animated with the phase information. It is meaningless and impossible to plot the real and imaginary components, as the animation requires the phase difference between different points in the structure. It is prudent to limit the frequencies of excitation so as to limit the amount of output. 362 Structural Engineering Analysis and Design Second Edition 4.5.3.1.1 Applied Load Excitations To define a frequency dependent dynamic excitation, both spatial distribution and the frequency variation (i.e. the temporal distribution) must be defined. The RLOAD1 entry defines dynamic excitation in real and imaginary format whilst the RLOAD2 entry defines dynamic excitation in magnitudes and phases. It is important to realize that P(f) is defined with the right-hand-side of the equation of motion in the frequency domain being Real [P(f)ei2πft]. Hence P(f) is the complex loading function in the frequency domain. {P(f)} = {A[C(f)+iD(f)ei{θ − 2πfτ}]} {P(f)} = {AB(f)ei{ φ(f) + θ − 2πfτ}} Note that C(f) + iD(f) = B(f)ei φ(f) RLOAD1: RLOAD2: f = frequency in cycles per unit time A = amplitude scalar multiplier defined by DAREA for a DOF τ = time delay in an applied load defined by DELAY for a DOF θ = phase lead angle in degrees defined by DPHASE for a DOF C(f) = frequency dependent real coefficient defined by Real TABLED1 D(f) = frequency dependent imaginary coefficient defined by Imaginary TABLED1 B(f) = frequency dependent amplitude curve defined by Amplitude TABLED1 φ(f) = frequency dependent phase angles curve in degrees defined by Phase TABLED1 $ CASE CONTROL SECTION DLOAD = < ID OF RLOAD1 or RLOAD2 > $ BULK DATA RLOAD1 ID DAREA ID DELAY ID DPHASE ID Real TABLED1 ID Imaginary TABLED1 ID RLOAD2 ID DAREA ID DELAY ID DPHASE ID Amplitude TABLED1 ID Phase TABLED1 ID DAREA ID GRID ID Component Number Scale Factor GRID ID Component Number Scale Factor DELAY ID GRID ID Component Number Time Delay τ GRID ID Component Number Time Delay τ DPHASE ID GRID ID Component Number Phase Lead θ (degrees) GRID ID Component Number Phase Lead θ (degrees) TABLED1 ID XAXIS YAXIS x1 y1 x2 y2 x3 y3 x4 x5 y5 x6 y6 … … ENDT 363 Y4 Structural Engineering Analysis and Design Second Edition Any number of DAREA, DELAY and DPHASE entries may be defined. All those with the same ID will be subjected to the dynamic excitation definition of Real/Amplitude TABLED1 and Imaginary/Phase TABLED1 as defined within the same RLOAD1/RLOAD2 entry. The XAXIS and YAXIS in the TABLED1 entry refers to either LINEAR or LOG interpolation between and beyond the extremities of the specified {xi , yi} pairs of {frequency, amplitude} or {frequency, phase angles}. Note that the frequencies are specified in cycles per unit time and the phase angles are specified in degrees. In order to verify the applied loading, the response at 0.0 Hz without structural damping should be checked to match the results from a static analysis, the discrepancy arising from mode truncation. It must be understood that use of complex numbers is only to ease mathematical manipulation. The harmonic excitation is understood to consist only of the real component of the complex number and likewise with the response. At a component of a DOF, [ ] = Re al[A (C + iDe ( P( t ) = Re al P(ω)e iωt where P(ω) is complex i θ −ωτ ) )e ] iωt If we required a simple P(t) = 1.0sinωt loading function, Let A = 1.0, D = −1.0 and all else zero, so that [( = Re al[− ie ] ) ] P( t ) = Re al 1 0 − i1e i (0−ω0 ) e iωt iωt = Re al[− i(cos ωt + i sin ωt )] = Re al[− i cos ωt + sin ωt ] = sin ωt If we required a simple P(t) = 1.0cosωt loading function, Let A = 1.0, C = 1.0 and all else zero, so that [( = Re al[1e ] ) ] P( t ) = Re al 1 1 − i0e i (0−ω0 ) e iωt iωt = Re al[1(cos ωt + i sin ωt )] = Re al[cos ωt + i sin ωt ] = cos ωt If we require P(t) = 1.0sinωt + 1.0cosωt, Let A = 1.0, C = 1.0, D = −1.0 and all else zero, so that [( ) ] = Re al[1(1 − i )e ] P( t ) = Re al 1 1 − i1e i (0−ω0 ) e iωt iωt = Re al[(1 − i )(cos ωt + i sin ωt )] = Re al[cos ωt + i sin ωt − i cos ωt + sin ωt ] = sin ωt + cos ωt 364 Structural Engineering Analysis and Design Second Edition Notice that cosωt is basically 90 degrees out of phase with sinωt. If we require a function which is out of phase by α, for instance P(t) = 1.0sin(ωt+α), Let A = 1.0, D = −1.0, θ = α and all else zero, so that [( = Re al[− ie ( ) ] P( t ) = Re al 1 0 − i1e i (α −ω0 ) e iωt i ωt +α ) ] = Re al[− i(cos(ωt + α ) + i sin (ωt + α ))] = Re al[− i cos(ωt + α ) + sin (ωt + α )] = sin (ωt + α ) Likewise, the steady-state response should be interpreted. [ u ( t ) = Re al F(ω)e iωt ] where F(ω) is complex  p   = Re al  D(ω) 0 e −iθ e iωt  k    p   = Re al D(ω) 0 e i (ωt −θ )  k   p   = Re al D(ω) 0 (cos(ωt − θ ) + i sin (ωt − θ)) k   p = D(ω) 0 cos(ωt − θ) k It is suggested that the P(ω) be inputted in Complex Cartesian format (i.e. RLOAD1) and that the response u(t) be interpreted in Complex Polar format. Remember that it is P(ω) that is inputted in RLOAD1 (and not P(t)) and that it is F(ω) which is outputted by NASTRAN in terms of preferably magnitude and phase. The NASTRAN output is p Phase = θ Magnitude = D(ω) 0 and k Note that D(ω) is the (magnitude of the) dynamic amplification factor. F(ω) can of course still be outputted in real and imaginary components if desired, but it is far more indicative if it is outputted in terms of magnitude and phase. All instances of phase refer to the clockwise angle from the real axis in the complex plane. Hence, we can make the following conclusions from the steady-state harmonic analysis, (i) (ii) (iii) if P(ω) is only positive real such that P(t) = 1.0cosωt, then the response will be p u ( t ) = D(ω) 0 cos(ωt − θ) k which means that the response lags the loading by θ. There will be a phase lag if and only if there is damping within the system. if P(ω) is only negative imaginary such that P(t) = 1.0sinωt, then the response will be p u ( t ) = D(ω) 0 sin (ωt − θ) k which means that the response again lags the loading by θ. There will be a phase lag if and only if there is damping within the system. if P(ω) is both real and imaginary, such that P(t) = 1.0sinωt + 1.0cosωt, then the response will be p u ( t ) = D(ω) 0 [sin(ωt − θ) + cos(ωt − θ)] k which means that the response again lags the loading by θ. There will be a phase lag if and only if there is damping within the system. Thus, it can be concluded that there will only be a phase lag in the response if there is damping within the system. 365 Structural Engineering Analysis and Design Second Edition Defining the spatial distribution using DAREA only enables the specification of dynamic concentrated forces and moments. To accommodate more complicated loadings, the LSEQ entry is used to refer to static load entries that define the spatial distribution of the dynamic loads. $ CASE CONTROL SECTION LOADSET = < ID OF LSEQ > DLOAD = < ID OF RLOAD1/RLOAD2 > $ BULK DATA LSEQ ID RLOAD1 ID RLOAD2 ID DAREA Reference Link DAREA Reference Link DAREA Reference Link Static Load ID Temp Load ID DELAY ID DPHASE ID DELAY ID DPHASE ID Real TABLED1 ID Amplitude TABLED1 ID Imaginary TABLED1 ID Phase TABLED1 ID The DAREA Reference Link links the RLOAD1/RLOAD2 entry to the LSEQ which can now be used to refer to static load set ids which define the spatial distribution of the dynamic loads. The static load set id can refer to one or more static load entry types. Obviously, there is not a DAREA entry anymore. It is replaced by an LSEQ bulk data entry, a LOADSET case control entry and the pertinent bulk data static load entries such as FORCE, PLOADi or GRAV. A new automatic feature will be activated if and only if the user does not have a LOADSET/LSEQ selection. With the new enhancement, it is no longer necessary for the user to explicitly specify LOADSET/LSEQ combination in order to employ static loading data in dynamic analysis. Instead, when the user selects a dynamic load, all static loads and thermal loads that have the same ID as the DAREA ID on the dynamic load entry are automatically selected. The frequency dependent load card RLOAD1/RLOAD2 is selected using the DLOAD case control command. If more than one RLOAD1/RLOAD2 entry is required, then a dynamic load set combination is required. This is done using a DLOAD bulk data entry that linearly combines multiple RLOAD1/RLOAD2 entries. $ CASE CONTROL SECTION DLOAD = < ID OF DLOAD > $ BULK DATA DLOAD ID Overall Scale Factor Scale Factor RLOAD1 / RLOAD2 ID 366 Scale Factor RLOAD1 / RLOAD2 ID ..etc.. Structural Engineering Analysis and Design Second Edition 4.5.3.1.2 Enforced Motion Four methods can be used for enforced motion, namely: (i) The direct absolute response approach (ii) The direct relative response approach (iii) The indirect large mass method (absolute response approach) (iv) The indirect large spring method (absolute response approach) The direct absolute response approach makes no assumptions. The direct relative response approach makes the following assumptions 3: (i) (ii) (ii) base movements in any given direction are identical i.e. that the base supports cannot move independently no mass or damping coupling between the structure and the ground (the off diagonal terms in the unsupported mass matrix that couple the structure and the ground movements are zero or are insignificant) no damping into the ground In both the direct absolute and direct relative approaches, the equation of motion is the same on the LHS, hence the same resonant frequencies and mode shapes are obtained, only the applied loading vector on the RHS differ. The two approaches will also give the same stresses within the elements. With the assumption of no coupling of mass and damping, the absolute response is found by applying a base displacement and the relative response by applying a base displacement. The absolute displacement response and relative displacement response only differ by a rigid body movement. 4.5.3.1.2.1 Direct Enforced Motion (Absolute Response Approach) The direct approach of applying enforced motion is the most accurate method. Denoting the free DOFs as f and the constrained DOFs (whether with enforced motion or zero constraints) as s, P the force and q the reaction, the dynamic equilibrium equation can be partitioned as With zero constraints, i.e. the dynamic equation of motion reduces to the usual with the corresponding reactions But, with enforced motion, the dynamic equation of motion is with the corresponding reactions 3 NAFEMS. A Finite Element Primer. NAFEMS Ltd., Great Britain, 1992. 367 Structural Engineering Analysis and Design Second Edition Hence, in general the user specifies the either the support displacement, velocity or acceleration, as all three motions are related to each other in the sense that the velocity is the first derivative and the acceleration is the second derivative of the displacement. But for most structural problems, the damping component Bsf (not Bss in the reaction expression) can be ignored and for lumped mass formulations (or at least no coupling to the support freedoms), Msf is zero, hence reducing the equivalent forcing function to Pf(t) – Kfs us(t) and hence, only the base displacement excitation needs to be incorporated. However, these approximations need not necessarily be employed in which case the absolute approach has no inherent assumptions. Note that the response will be obtained in absolute terms. This solution method is general and is valid even if different supports are moving with different independent excitations. 4.5.3.1.2.2 Direct Enforced Motion (Relative Response Approach) Described for the time domain in the direct transient response section. The DLOAD Case Control Command, optionally the DLOAD bulk data entry, RLOAD1/RLOAD2, DELAY, DPHASE and TABLED1 is used in the same way as they were when load excitations were applied. One difference is the TYPE Field 8 of RLOAD1/RLOAD2 where enforced motion in terms of DISP, VELO or ACCE is specified. Another difference for the direct enforced motion lies in the EXCITEID Field 3 of RLOAD1/RLOAD2, where instead of referencing a DAREA card (hence not requiring a DAREA card at all for enforced motion), the EXCITEID Field references an SPCD entry, which in turn will reference a GRID ID and an associated DOF component in which the enforced motion is to be applied. Now at the same time, in line with methods of applying enforced motion in static analysis, the DOF component of the GRID ID with enforced motion must be constrained with an SPC bulk data entry which of course must be referenced by an SPC Case Control Command. Modal augmentation vectors by PARAM, RESVEC, YES must be used for modal methods. This is because since there no rigid body modes (as they are constrained by the enforced motion), there can be no motion of the enforced points unless RESVEC is used. 368 Structural Engineering Analysis and Design Second Edition 4.5.3.1.2.3 Indirect Large Mass Method (Absolute Response Approach) – Base Acceleration Specified If a very large mass m0, which is several orders of magnitude larger than the mass of the entire structure, is connected to a DOF where a dynamic load is applied, then the acceleration of the DOF is approximately P(t ) & u&( t ) = m0 Hence, the (large) force required to produce the desired acceleration at the DOF is P( t ) = m 0 & u&( t ) The stiffness, damping and the inertial force of the mass of the structure at the DOF contributes little in comparison to the force provided by the large mass, hence the acceleration response is due primarily to the inertial force of the large mass. The larger the mass in comparison, the more accurate the acceleration excitation. However the magnitude is limited by numeric overflow in the computer. MSC recommends that the value of m0 be approximately 106 times the mass of the entire structure for an enforced translational DOF and 106 times the mass moment of inertia of the entire structure for a rotational DOF (for 6 digits of numerical accuracy). The disadvantage of the large mass method is that it involves a loss of numerical conditioning and hence a loss of accuracy of the response. If the large mass is 106 times the mass of the structure, this is equivalent to losing 6 significant figures in the definition of the mass and stiffness matrices. The following procedure is employed to specify prescribed motion in forced frequency response analysis: (i) remove constraints from the enforced DOFs (ii) place large masses or inertia scalar elements CMASSi or CONMi with values approximately 106 times the mass or mass moment of inertia of the entire structure (iii) if a sinusoidal displacement motion is to be prescribed Prescribed displacement u ( t ) = B sin( 2πft ) Hence, prescribed acceleration & u&( t ) = − B4π 2 f 2 sin(2πft ) Hence, load with large mass method P(t) = P(f) sin( 2πft ) = − m 0 B4π 2 f 2 sin( 2πft ) Hence, P(f) = − m 0 B4π 2 f 2 Clearly, if a sinusoidal (of amplitude B) velocity or acceleration was to be prescribed the amplitude of the force P(f) would simply be m0B2πf or m0B respectively. The scale factor A=Bm0 can be entered in the DAREA entry. The factors –4π2f2 and 2πf are frequency-dependent factors which has to be entered using the TABLED4 entry, illustrated for the former as follows, TABLED4 ID X1=0.0 X2=1.0 X3=0.0 X4=10000.0 A0=0.0 A1=0.0 A2=−4π2 A3 A4 The TABLED4 entry has the following algorithm, y= N ∑ i =0  x − X1  Ai    X2  i In this case,  x − 0 .0  y = −4 π 2    1 .0  2 369 A5 … etc … ENDT Structural Engineering Analysis and Design Second Edition Only the coefficient A2 is of a non-zero value to generate a frequency dependent coefficient to the second degree. Likewise a prescribed sinusoidal velocity will have a frequency dependency to the first degree and a prescribed sinusoidal acceleration will not have a frequency dependency. Note that when x < X3, x = X3 and when x > X4, x = X4. This has the effect of placing bounds on the table, there is no extrapolation outside the table boundaries. ENDT ends the table input. The DLOAD Case Control Command, optionally the DLOAD bulk data entry, RLOAD1/RLOAD2, DAREA, DELAY, DPHASE and TABLED1 is used in the same way as they were when load excitations were applied. To ensure that the chosen mass values are high enough two modal analyses (SOL 103) should be run, one with the enforced DOFs constrained and the other with the large masses attached and the DOFs left unconstrained. The flexible frequencies (not the rigid mode frequencies) between the two analyses should be well comparable (to within 4 or 5 significant figures), otherwise the mass values should be increased. In modal methods, further considerations must be made to the rigid body modes. Globally unconstrained structures will have rigid body modes. Releasing a global DOF and placing a large mass there to enforce an applied motion will result in that DOF being unconstrained and hence will result in a rigid body mode (stress free mode). This mode can safely be discarded in the solution by using LFREQ or simply not calculating it in EIGRL. If however two large masses are placed at two different locations to simulate enforced motion in the same direction, there will be a further low-frequency mode that represents the motion of one large mass relative to the other. This mode does contribute to the stresses are cannot be ignored. It must be captured within EIGRL and LFREQ. To avoid this problem, a solution will be to place only one large mass at an arbitrary location and connect with RBE2 elements all DOFs that are to be subjected to that enforced motion. 4.5.3.1.2.4 Indirect Large Spring Method (Absolute Response Approach) – Base Displacement Specified Described for the time domain in the direct transient response section. 370 Structural Engineering Analysis and Design Second Edition 4.5.3.2 GL, ML P-∆ (KGA From KEA) Direct Forced Frequency Response Analysis It is often necessary to incorporate the reduction in bending stiffness of gravity load resisting columns for the analysis of lateral loads. The following procedure is undertaken. Phase 1 Perform static analysis (with loads that cause the greatest negative or positive geometric stiffness) based on [KEA] but include the segyroa.v2001 alter prior to the Case Control Section in order to compute the geometric stiffness matrix [KGA]1 (and output into a .pch file) based on the generated element loads from the [KEA] static analysis. Phase 2 A SOL 108 is undertaken based on [KEA] + [KGA]1 with the k2gg=ktjj statement in the Case Control Section and the outputted .pch file which contains the ktjj matrix in the Bulk Data. The responses at this stage represent the P-∆ (KGA From KEA) response to the dynamic excitation. The following equivalent alternative procedure can also be employed. $ CASE CONTROL SECTION SUBCASE 1 LABEL = Static Preload Load Case LOAD = < ID of FORCEi, MOMENTi, PLOADi, GRAV, LOAD, SPCD Cards in Bulk Data > TEMP(LOAD) = < ID of TEMP, TEMPRB, TEMPP1 Cards in Bulk Data > DEFORM = < ID of DEFORM Cards in Bulk Data > SUBCASE 2 LABEL = P-∆ Direct Frequency Response Analysis STATSUB(PRELOAD) = 1 DLOAD = < ID OF RLOAD1 or RLOAD2 > The method is valid when only the prestress is judged to affect the geometric stiffness such as in the compressive preload of building columns due to gravitational loads and the prestressing of extremely taut cables that sag very little under gravity but not in systems such as suspension bridges. Where lateral loads are large enough to affect the geometry of the system with prestress, then a repetitive P-∆, SOL 106, implicit dynamic relaxation SOL 129 or explicit dynamic relaxation must be employed. But in single P-∆ analysis, because cables do not have much elastic bending stiffness, the initial static preload subcase should only include the prestress and not gravity as including gravity is the same as solving two linear static problems of stiffness KEA with preload and gravity as the applied loads respectively. Clearly, in the gravity case, it is nonsensical as the cables do in reality have differential stiffness (from the prestress) to resist the gravitational force. Prestress in one direction (i.e. along the axis of cable) will cause a differential stiffness in the orthogonal direction. Gravity acts in the orthogonal direction and hence cannot be accounted for in the calculation of the prestress in this single P-∆ analysis. To quantitatively decide if gravity need not be considered in contributing to the differential stiffness of the cables, a static P-∆ analysis should be carried out, the first subcase being a SOL 101 with only the prestress as applied loads and the second subcase a P-∆ SOL 101 (i.e. utilizing the induced prestress from the first subcase to form a geometric stiffness matrix) with both the gravity and prestress included as applied loads. If the difference in the cable element forces between subcases 1 and 2 is negligible, then gravity has little influence in affecting the geometric stiffness. If there is a major difference in the cable element force, then clearly, gravity will affect the geometric stiffness and as such, a repetitive P-∆ , SOL 106, implicit dynamic relaxation or explicit dynamic relaxation must be used to converge to the true KT. Likewise, in the single P-∆ analysis of multi-storey buildings, gravity (and only gravity) acts in axis of columns to generate prestress, and the differential stiffness is computed for the orthogonal direction reducing resistance to lateral wind forces, applied in the second subcase with gravity too. 371 Structural Engineering Analysis and Design Second Edition When a static subcase is specified for linear transient response analysis (SOLs 109 and 112) with STATSUB(PRELOAD), the data recovery is controlled by PARAM, ADSTAT. By default (YES) the static solution will be superimposed on the dynamic response solution (displacement, stress and SPCForce). The relative solution can be obtained in reference to the static solution point by PARAM, ADSTAT, NO. No provision is made for frequency response analysis, because the static responses contribute only to the zero frequency response. The STATSUB(PRELOAD) computes the differential stiffness due to the prestress and also the follower force. The follower force is calculated and incorporated by the use of PARAM, FOLLOWK, YES. We know how the prestress affects the differential stiffness, namely a tensile prestress causing an increase in stiffness. The effect of the follower force on the stiffness is different. For example, for a cylinder under external pressure critical buckling load may be overestimated (even though the mode shapes are similar) in a SOL 105 and the natural frequencies in vibration may be underestimated (even though the mode shapes are similar) in a SOL 103 in the absence of follower stiffness. To the contrary, these observations are reversed in case of centrifugal loads. Centrifugal forces as a constant (static) load are applied by a Bulk Data RFORCE to any elements that have masses. The follower stiffness due to centrifugal load has the effect of lowering stiffness (although the centrifugal load tensioning effect increases stiffness), consequently lowering natural frequencies (even though the mode shapes are similar) in a SOL 103 and lowering the buckling loads (even though the mode shapes are similar) in a SOL 105. This effect increases as the RPM increases, and it becomes significant when the RPM is over 1000. For moderately geometric nonlinear analysis, exclusion of follower stiffness affects the rate of convergence, but the converged solution is correct. For severely geometric nonlinear analysis, it may not be possible to obtain a converged solution without including follower stiffness. As the geometric nonlinearity intensifies, so is the effect of follower stiffness. Therefore, inclusion of follower stiffness greatly enhances the convergence if the deformation involves severe geometric nonlinearity. 372 Structural Engineering Analysis and Design Second Edition 4.5.3.3 GL, ML P-∆ (KGA From Exact or Approximate KTA) Direct Forced Frequency Response Analysis It is often necessary to include the differential stiffness, especially if there are prestressed cables in the model. To obtain KTA, to be theoretically exact, a GNL SOL 106 (or implicit dynamic relaxation SOL 129 or explicit dynamic relaxation LS-DYNA) with prestress (as temperature loads say) and gravity must be undertaken. Alternatively, an approximation to KTA can be obtained by repetitive P-∆ static analyses with the prestress (as temperature loads say) and gravity applied. The procedure to obtain this approximate KTA will be presented. Note that the approximate KTA will be the summation of the elastic stiffness KE at the undeflected (by the prestress and gravity) state but KG at the deflected (by the prestress and gravity) state. Hence if KE changes considerably during the application of the prestress, a full SOL 106 (or implicit dynamic relaxation SOL 129 or explicit dynamic relaxation LS-DYNA), which converges to the KE and KG at the deflected (by the prestress and gravity) state should be employed. Hence for the modelling of a suspension bridge where there is a great change in geometry (known in the bridge industry as form-finding, so-called because it is necessary to find the form or shape of the catenary suspension cables), it may be prudent to employ SOL 106 (or implicit dynamic relaxation SOL 129 or explicit dynamic relaxation LSDYNA), but for a high tension low sag cable on say a tower with prestressed cables, the repetitive P-∆ static analysis may be adequate. The repetitive P-∆ analysis basically involves a number of iterations of linear static analyses to obtain an approximate KTA. Note again that A refers to the initial undeflected (by the collapsing load) state, but deflected by the prestress and gravity. To perform the repetitive P-∆ analysis, a static analysis is performed based on KEA with temperature loads and gravity to generate forces in the structural elements, which in turn provides input for the computation of KGiAKTm where m is the iterations. Repetitive static analysis is performed with the prestress and gravity updating the stiffness matrix KEA + KGiAKTm-1 + KGiAKTm until convergence of displacements is obtained. The tangent stiffness at this stage is the approximate converged tangent stiffness matrix KTA = KEA + KGiAKT. The converged displacements represent the approximate P-∆ (KGA From Approximate KTA) static response to the initial prestress loads. The converged geometric stiffness at this stage would be that based upon the approximate tangent stiffness matrix KTA, i.e. KGiAKT. Phase 1 Perform static analysis (with prestress and gravity) based on [KEA] but include the segyroa.v2001 alter prior to the Case Control Section in order to compute the geometric stiffness matrix [KGA]1 (and output into a .pch file) based on the generated element loads from the [KEA] static analysis. Phase 2 Perform static analysis (with prestress and gravity) based on [KEA] + [KGA]1 by including the k2gg = ktjj statement in the Case Control Section, the outputted .pch file which contains the ktjj matrix in the Bulk Data and the segyroa.v2001 alter prior to the Case Control Section to compute the [KGA]2 (and output into the .pch file overwriting previous data) based on the generated element loads from the [KEA] + [KGA]1 static analysis. Phase 3 Repeatedly perform the Phase 2 static analysis (with prestress and gravity) based on [KEA] + [KGA]i for i = 2 to n where n represents the number of iterations required for the change in deflections between analyses to become negligible. This would signify that the change in the [KGA] matrix become negligible and the correct [KGA] is attained. The deflections and the other responses at this stage represent the P-∆ (KGA From Approximate KTA) static response to the prestress and gravity. The stiffness of the structure is KTA. Phase 4 A SOL 108 is undertaken with the k2gg=ktjj statement in the Case Control Section and the outputted .pch file which contains the latest ktjj matrix in the Bulk Data. The responses at this stage represent the P-∆ (KGA From Approximate KTA) response to the dynamic excitation. 373 Structural Engineering Analysis and Design Second Edition 4.5.4 4.5.4.1 Hand Methods Verification The Theory of the Dynamic Magnification Factor for Undamped Motion and Hence the Determination of Maximum Dynamic Displacement, umax for Deterministic Harmonic Loading by Classically Solving the SDOF Linear Undamped ODE and Maximizing the Solution Equation of motion [ m& u&( t ) + ku ( t ) = Re al p 0 e iωt ] Assume solution u(t) = u c (t) + u p ( t ) For homogenous part, m& u&c ( t ) + ku c ( t ) = 0 [ ] assume u c (t) = Re al Ge λt where G = G R + iG I and λ = α + iωd 2 λt λt mGλ e + kGe = 0 (mλ ) (mλ +k =0 + k Ge λt = 0 for LHS to be zero for all t 2 2 ) Ge λt > 0 as the roots of this quadratic characteristic equation are λ1 = +i k m λ 2 = −i ∴α = 0 k m ωd = ω n = and hence, the complementary function, [ u c (t) = Re al G 1e λ1t + G 2 e λ 2 t k rad / s m ] u c (t) = Re al [(G 1R + iG 1I )(cos ωn t + i sin ω n t ) + (G 2 R + iG 2 I )(cos ωn t − i sin ω n t )] u c ( t ) = Re al [((G1R + G 2 R )cos ω n t − (G1I − G 2 I )sin ωn t ) + i((G 1I + G 2 I ) cos ω n t + (G1R − G 2 R )sin ωn t )] for the free vibration response to be real for all t, G 1I = −G 2 I and G 1R = G 2 R sin ce there are two less independent constants, let G 1I = −G 2 I = G I and G 1R = G 2 R = G R we notice that G 1 and G 2 are a complex conjugate pair G 1 = G R + iG I and G 2 = G R − iG I hence u c ( t ) = 2G R cos ω n t − 2G I sin ωn t For the inhomogenous part, [ ] assume u p ( t ) = Re al F(ω)e iωt , hence on substituti on, − mω F(ω) + kF(ω) = p 0 2 F(ω) = p0 p0 / k = k − mω 2 1 − (ω / ω n ) 2 thus [ ] u p ( t ) = Re al F(ω)e iωt = p0 / k cos ωt 1 − (ω / ω n ) 2 374 Structural Engineering Analysis and Design Second Edition Hence, the general solution is u ( t ) = 2G R cos ω n t − 2G I sin ω n t + where 2G R = p0 / k cos ωt 1 − (ω / ω n ) 2 ωp 0 / k u&(0) − ωn 1 − ω 2 / ω 2n ω n ( ) and −2G I = u (0) Notice that the initial conditions were obtained from the general solution, and not from considering the complementary function alone. Investigating the frequency of the response, the starting transient solution uc(t) is at the frequency and is in phase with the structure’s ωn, whilst the steady-state solution up(t) is at the frequency and is in phase with the loading’s ω. Since there is no damping, there is no imaginary component in the complex response function F(ω). Investigating the amplitude of the response, the steady-state solution has a static displacement amplitude p0/k scaled by the (magnitude of the) dynamic amplification factor 1/(1−ω2/ωn2). Hence, the (magnitude of the) dynamic amplification factor D(ω) increases as ω/ωn approaches unity, and resonance occurs. With no damping, the maximum (magnitude of the) dynamic amplification occurs exactly when ω = ωn. 375 Structural Engineering Analysis and Design Second Edition 4.5.4.2 The Theory of the Dynamic Magnification Factor for Damped Motion and Hence Determination of Maximum Dynamic Displacement, umax for Deterministic Harmonic Loading by Classically Solving the SDOF Linear Damped ODE and Maximizing the Solution Equation of motion [ m& u&( t ) + cu&( t ) + ku ( t ) = Re al p 0 e iωt m& u&( t ) ] p0eiwt ku(t) Assume solution u(t) = u c (t) + u p ( t ) m For homogenous part, m& u&c ( t ) + cu&c ( t ) + ku c ( t ) = 0 [ u(t) cu&( t ) ] assume u c (t) = Re al Ge λt where G = G R + iG I and λ = α + iωd 2 λt λt mGλ e + cGλe + kGe λt = 0 (mλ ) + cλ + k Ge λt = 0 for LHS to be zero for all t 2 (mλ 2 ) + cλ + k = 0 Ge λt > 0 as the roots of this quadratic characteristic equation are 2 c k  c  +   − 2m 2 m m   hence, the complementary function, 2 λ1 = − [ u c (t) = Re al G 1e λ1t + G 2 e λ 2t λ2 = − c k  c  −   − 2m 2 m m   ] in the under - damped case, c < c cr , the roots are complex conjugates, k  c  c +i −  m  2m  2m employing Euler's equations, λ1 = − 2 λ2 = − k  c  c −i −  m  2m  2m 2 e iθ = cos θ + i sin θ e −iθ = cos θ − i sin θ hence, writing ωd = k  c  −  m  2m  2 c c   − − t t u c ( t ) = Re al (G 1R + iG 1I )e 2m (cos ωd t + i sin ωd t ) + (G 2 R + iG 2 I )e 2 m (cos ωd t − i sin ωd t )    −ct  u c ( t ) = Re al e 2 m [((G 1R + G 2 R )cos ωd t − (G 1I − G 2 I )sin ωd t ) + i((G 1I + G 2 I )cos ωd t + (G 1R − G 2 R )sin ωd t )]   for the free vibration response to be real for all t, G 1I = −G 2 I and G 1R = G 2 R sin ce there are two less independent constants, let G 1I = −G 2 I = G I and G 1R = G 2 R = G R we notice that G 1 and G 2 are a complex conjugate pair G 1 = G R + iG I and G 2 = G R − iG I hence u c (t) = e − c t 2m [(2G R cos ωd t − 2G I sin ωd t )] 376 Structural Engineering Analysis and Design Second Edition defining the damping ratio ζ such that c = ζc cr = ζ 2 km = ζ 2mω n the damped natural circular frequency, 2 ωd = k  ζ 2 km  − = m  2m  ( k ζ 2k − = m m ) k 1 − ζ 2 = ωn 1 − ζ 2 m hence, the complementary function u c ( t ) = e −ζωn t [(2G R cos ωd t − 2G I sin ωd t )] where ωd = ω n 1 − ζ 2 and 2G R , − 2G I being the constants of integration from the initial conditions. For the inhomogeno us part, [ ] assume u p ( t ) = Re al F(ω)e iωt , hence on substituti on, -mω 2 F(ω) + icωF(ω) + kF(ω) = p 0 p0 k − mω 2 + icω from complex number theory F(ω) = x + iy =  x 2 + y 2 e iθ , θ = tan −1 ( y / x )   changing the denominato r to a polar complex form F(ω) = F(ω) = p0 (k − mω ) + (cω)2 e iθ 2 2 (1 − ω thus, p0 / k 2 / ωn ) 2 2 [ u p ( t ) = Re al F(ω)e iωt u p (t) = , θ = tan −1 (1 − ω / ωn ( e −iθ , θ = tan −1 + (2ζω / ω n ) 2 2ζω / ω n (1 − ω 2 / ωn 2 ) ) ] p0 / k 2 2ζω / ω n cω = tan −1 2 2 k − mω 1 − ω2 / ωn ) 2 2 cos(ωt − θ) + (2ζω / ω n ) 2 Hence the general solution, u ( t ) = e −ζωn t [(2G R cos ω d t − 2G I sin ω d t )] + where ω d = ω n 1 − ζ 2 , θ = tan −1 p0 / k (1 − ω 2 ω 2n ) 2 + ( 2ζω / ω n ) 2 cos(ωt − θ) 2ζω / ω n (1 − ω 2 ω 2n ) The starting transient is insignificant because the term e−ζωnt will cause it to vanish. Investigating the frequency of the response, the insignificant starting transient is at the damped natural frequency of the structure, ωd = ωn(1-ζ2)1/2 and the steady-state solution is at the frequency of but out of phase with the loading’s ω by θ. The complex response function F(ω) may contain both real and imaginary components depending on the complex loading function P(ω) and the existence of damping within the system, i.e. (i) If P(ω) is real and there is no damping within the system, F(ω) is real (ii) If P(ω) is complex and there is no damping within the system, F(ω) is complex (iii) If P(ω) is real and there is damping within the system, F(ω) is complex (iv) If P(ω) is complex and there is damping within the system, F(ω) is complex 377 Structural Engineering Analysis and Design Second Edition The complex expression for F(ω) is often expressed in magnitude and phase θ. If P(ω) is only real, the value of the phase angle θ gives an indication of the damping inherent within the system. Recapping basic complex number theory, a complex number contains real and imaginary components z = x + iy it can be written in a polar form by computing the magnitude and the phase z =  x 2 + y 2 e iθ ,   θ = tan −1 ( y / x ) z =  x 2 + y 2 (cos θ + i sin θ), θ = tan −1 ( y / x )   The Cartesian form is visualized on a Cartesian diagram of real x- and imaginary y-axes. The polar form is visualized on the same Cartesian diagram with the magnitude being the radius from the origin and the phase being the angle of the radius from the real x-axis. It is implicitly understood that when a complex vector is used to represent a harmonic motion, it is the horizontal projection of the complex vector (i.e. the real component) that represents the motion. Investigating the amplitude of the response, the steady-state solution has a static displacement amplitude p0/k scaled by the (magnitude of the) dynamic amplification factor, D(ω). D(ω) = (1 − ω 1 2 / ωn ) 2 2 + (2ζω / ω n ) 2 The following cases are identified: (i) If ω/ωn << 1 (very low frequency loading), the (magnitude of the) dynamic amplification D(ω) approaches 1, stiffness forces dominate and static solution obtained with the displacement response in phase with loading. Performing a frequency response analysis at a frequency of 0.0 Hertz gives the same results as a static analysis. The phase angle θ approaches 0°. (ii) When ω = ωn, the (magnitude of the) dynamic amplification factor D = 1/(2ζ). Resonance by definition occurs. Stiffness and inertial forces cancel each other and applied force is balanced by damping (hence the greater the damping, the smaller the response). Although the maximum amplification is not at its greatest, it is close enough to the maximum for even moderate amounts of damping. The phase angle θ is 90°. (iii) If ω/ωn = (1-2ζ2)1/2 (note how this is slightly different from ωd = ωn(1-ζ2)1/2 meaning which the maximum amplification does not actually occur exactly when the forcing frequency equals the damped natural frequency, never mind the undamped natural frequency, ωn), the maximum (magnitude of the) dynamic amplification occurs. D = 1/(2ζ(1−ζ2)0.5). (iv) If ω/ωn >> 1 (very high frequency loading), the (magnitude of the) dynamic amplification D(ω) approaches 0, inertial forces dominate and no displacement obtained, i.e. loading is changing too fast for the structure to respond. The displacement response will be 180° out of phase with loading (i.e. displacement response will have opposite sign to loading force). Hence, the increase in maximum response for a dynamic analysis compared to a static analysis comes from the (magnitude of the) dynamic amplification factor, which is a function of the forcing amplitude and the ratio between the forcing frequencies and the natural frequencies. If the structure is excited close to a resonance, then the stiffness force (potential or strain energy) and the inertia forces (kinetic energy) cancel out and the response amplitude is greater in order to maintain equilibrium. The amplitude of vibration is then controlled by the level of damping. The external forces are balanced by the damping forces. The frequencies at which resonance occurs, that is when the stiffness and the inertia forces cancel are called the natural frequencies of the system. This is evident from the eigenvalue problem [K]{φ} = ω2[M]{φ} where frequencies are found such that the inertia and stiffness forces cancel. It is the frequencies at which a free undamped system will vibrate if disturbed from equilibrium. Damping 378 Structural Engineering Analysis and Design Second Edition causes the peak amplitude to occur at a slightly lower frequency so that the damped resonant frequency is slightly lower than the undamped natural frequency, but since typical structures are under-damped this change is so small it can be neglected. If the system is excited at some frequency other than resonance, then the amplitude of the response is largely controlled by the stiffness and inertia forces. In this case, they do not cancel each other and so the damping force is generally not as significant. When damping is not considered, the maximum (magnitude of the) dynamic amplification occurs at resonance when the forcing frequency, ω exactly matches the natural circular frequency, ωn. In that case, the amplification is infinite. This is not the case when damping is considered, i.e. maximum (magnitude of the) dynamic amplification does not occur exactly at resonance when the forcing frequency, ω matches the natural circular frequency, ωn or when ω matches the damped natural circular frequency, ωd = ωn(1-ζ2)1/2 for that matter, instead the maximum (magnitude of the) dynamic amplification occurs when ω = ωn(1-2ζ2)1/2. Variation of Phase Angle with Frequency Ratio For Different Damping 6 200 5 zhi=0 4 zhi=0.1 3 zhi=0.2 Phase Angle Dynamic Amplification Factor, D Variation of D with Frequency Ratio For Different Damping zhi=1 2 zhi=2 zhi=0 150 zhi=0.1 zhi=0.2 100 1 zhi=1 zhi=2 50 0 0 0 1 0 2 1 2 Frequency Ratio ω/ωn ω/ω Frequency Ratio ω/ωn ω/ω The shape of the (magnitude of the) dynamic amplification factor D(ω) versus frequency ratio ω/ωn depends on the level of damping, as of course does the maximum (magnitude of the) dynamic amplification. Dmax ≈ Dresonant = 1/(2ζ). D Dresonant /√2 1 ω (ω/ωn)1 ωn (ω/ωn)2 0 Measuring the bandwidth at 1/√2 of peak resonant amplitude for convenience, we can write for when 1 1 2 2ζ 1 1 1 = 2 2 2 2 2 2ζ (1 − ω ω n ) + ( 2ζω / ω n ) D resonant = 379 Structural Engineering Analysis and Design Second Edition Squaring both sides and solving for the frequency ratio, ( ω / ω n ) 2 = 1 − 2 ζ 2 ± 2ζ 1 + ζ 2 Ignoring higher order terms of ζ2, hence the assumption that this final equation is valid for only small damping ζ, ( ω / ω n ) 2 = 1 − 2 ζ 2 ± 2ζ ∴ (ω / ω n )12 = 1 − 2ζ 2 + 2ζ (ω / ω n ) 22 = 1 − 2ζ 2 − 2ζ ∴ (ω / ω n ) 1 = 1 + ζ − ζ 2 (ω / ω n ) 2 = 1 − ζ − ζ 2 Finally, subtracting one root from each other ζ= (ω / ω n ) 2 − (ω / ω n )1 ω 2 − ω1 f 2 − f 1 = = 2 2ω n 2f n Remember that only when damping is small that the maximum (magnitude of the) dynamic amplification can be approximated to occur at resonance, by definition when the forcing frequency equals the undamped natural frequency. When damping is high, it is imperative that the (magnitude of the) dynamic amplification expression be differentiated or use is made of ωd = ωn(1-2ζ2)1/2 as the point at which the maximum (magnitude of the) dynamic amplification occurs. 380 Structural Engineering Analysis and Design Second Edition 4.5.4.3 The Theory of Vibration (Base) Isolation and the Force Transmitted Into Rigid Foundation by the Damped Structure Subjected to Deterministic Harmonic Loading Knowing the displacement response of a linear damped SDOF system subjected to deterministic harmonic loading also means that we can derive the velocity response. This means that we can evaluate the force transmitted through the spring-damper system. Considering the steady-state response due to a harmonic excitation of p0sinωt, u ( t ) = D (ω) p 0 / k sin (ω t − θ ) where 1 D(ω) = (1 − ω 2 ω 2n ) 2 + ( 2ζω / ω n ) 2 and θ = tan −1 2ζω / ω n (1 − ω 2 ω 2n ) Hence the force in the spring - damper system Force ( t ) = ku ( t ) + cu&( t ) = D(ω) p 0 / k (k sin (ω t − θ ) + cω cos (ωt − θ )) = D(ω) p 0 / k k 2 + c 2 ω 2 sin (ω t − θ + β ) where tan β = cω /k = 2ζω / ω n = D(ω) p 0 1 + (2ζω / ω n ) sin (ωt − θ + β ) where tan β = cω /k = 2ζω / ω n Now, we define an expression for the relative transmissibility as the force response amplitude divided by the amplitude of the enforcing harmonic force, Tr = = Force Response Amplitude p0 Dp 0 1 + (2ζω / ω n )2 p0 1 + (2ζω / ω n ) 2 = (1 − ω 2 ω 2n ) 2 + ( 2ζω / ω n ) 2 This is the force transmissibility expression. It will be shown that this expression can also represent the displacement and acceleration transmissibility’s. This expression of force transmissibility is useful to calculate the force in the spring-damper system due to both stiffness and viscous damping. This can be used to calculate the force induced into a foundation by a vibrating structure. For instance, we can evaluate the force induced by a rotating machine into the supporting structure. And hence, we can design the supporting system of the rotation machine such that it induces the least amount of vibrations into the supporting structure (and hence the rigid foundation). The concepts behind vibration isolation (i.e. by investigating the transmissibility expression) is the same whether we are investigating (i) (ii) the force transmitted into the supporting structure (and hence the rigid foundation) due to a component subjected to harmonic force, or the displacement and acceleration response of a component subjected to harmonic displacement or acceleration at the rigid foundation On investigating the transmissibility expression, we can design the supporting system for vibration isolation. The transmissibility is unity when the supporting system is infinitely stiff with respect to the loading frequency. The transmissibility is also unity when the frequency ratio is √2. If the supporting system is designed such that the frequency ratio is less than √2 but greater than 0, the transmissibility is greater than one, which means that the supporting system actually makes matters worse as far as vibration isolation is concerned. When the frequency ratio is greater than √2, it is seen that the transmissibility is smaller than unity and hence, the supporting system 381 Structural Engineering Analysis and Design Second Edition functions as a vibration isolator. Damping is seen to be advantages only in the region when the frequency ratio is less than √2 (where a spring mounting supporting system makes matters worse) and not when the frequency ratio is greater than √2 (where a spring mounting supporting system acts as an effective vibration isolator). This is not so important actually as the undesirable effects of high values of damping at frequency ratios greater than √2 is not so great especially at even higher frequency ratios, i.e. achieved by making the supporting system even more flexible. Also, in the unfortunate circumstance that the resonance region of frequency ratio less than √2 is somehow attained; high levels of damping are extremely effective. For good isolation, it is often recommended to design the supporting system for a frequency ratio of at least 3. Note that the above force transmissibility expression is only valid if the foundation is rigid. If the foundation is not rigid, then the supporting system must be even more flexible in order to provide the same level of protection as when the foundation is rigid. 382 Structural Engineering Analysis and Design Second Edition 4.5.4.4 The Theory of Vibration (Base) Isolation and the Determination of Maximum Dynamic Displacement, umax for Deterministic Harmonic Support Motion (Displacement, Velocity or Acceleration) by Classically Solving the SDOF Linear Damped ODE (in Absolute and Relative Terms) and Maximizing the Solution If instead of a harmonic force, the SDOF dynamic system can be subjected to a harmonic displacement such as a support motion. Let us consider the equation of motion in absolute terms at first. m& u&( t ) k(u(t)- us(t)) m u(t) c(u&( t ) − u&s ( t ) ) us(t) = u0sinωt Equation of motion m& u&( t ) + c(u&( t ) − u&s ( t ) ) + k (u ( t ) − u s ( t ) ) = 0 Re placing u s ( t ) = u 0 sin ωt m& u&( t ) + cu&( t ) + ku ( t ) = ku 0 sin ωt + cωu 0 cos ωt m& u&( t ) + cu&( t ) + ku ( t ) = p 0 sin (ωt + β) where p 0 = u 0 k 2 + (cω) = u 0 k 1 + (2ζω / ω n ) 2 2 tan β = cω / k = 2ζω / ω n This equation is similar to that of the harmonic loading except that there is a phase angle β in the loading. Hence the steady state solution is also similar except for the addition of the β phase angle. p0 / k 2ζω / ω n θ = tan −1 u (t) = sin (ωt + β − θ ) 2 2 2 2 ( 1 − ω 2 ω 2n ) (1 − ω ω n ) + ( 2ζω / ω n ) But now, p0/k is not the static displacement any longer. Replacing the expression for p0 u 0 1 + (2ζω / ω n ) 2 u (t) = (1 − ω 2 ω 2n ) 2 + ( 2ζω / ω n ) 2 sin (ωt + β − θ ) θ = tan −1 2ζω / ω n (1 − ω 2 ω 2n ) The amplitude of the response is thus F= u 0 1 + (2ζω / ω n ) 2 (1 − ω 2 ω 2n ) 2 + ( 2ζω / ω n ) 2 Now, we define an expression for the relative transmissibility as the displacement response amplitude F divided by the amplitude of the enforcing harmonic displacement, Tr = F = u0 1 + (2ζω / ω n )2 (1 − ω 2 ω 2n ) 2 + ( 2ζω / ω n ) 2 This is the displacement transmissibility expression. The acceleration transmissibility is exactly similar. A plot of Tr versus ω/ωn is somewhat similar to that of (the magnitude of the) dynamic amplification D versus ω/ωn, except that all the curves of different ζ pass through the same point of Tr = 1.0 when ω/ωn = √2. Noting the curves after 383 Structural Engineering Analysis and Design Second Edition this point it is observed that damping tends to reduce the effectiveness of vibration isolation for frequency ratios greater than √2. Variation of Tr with Frequency Ratio For Different Damping Transmissibility, Tr 6 zhi=0 5 zhi=0.1 4 zhi=0.2 zhi=0.3 3 zhi=0.4 zhi=1.0 2 zhi=2.0 1 0 0 1 Frequency Ratio ω/ωn ω/ω 2 This formula is effective to determine the stiffness and damping (hence natural frequency) of an isolation system knowing the input displacement or acceleration and the maximum acceptable dynamic displacement or acceleration that the structural component can be subjected to. Remember that only when damping is small that the maximum transmissibility can be approximated to occur at resonance. When damping is high, it is imperative that the transmissibility expression be differentiated (also use cannot be made of ω = ωn(1-2ζ2)1/2 as this is based on differentiating and maximizing the (magnitude of the) dynamic amplification factor, D). On investigating the transmissibility expression, we can design the supporting system for vibration isolation. The transmissibility is unity when the supporting system is infinitely stiff with respect to the loading frequency. The transmissibility is also unity when the frequency ratio is √2. If the supporting system is designed such that the frequency ratio is less than √2 but greater than 0, the transmissibility is greater than one, which means that the supporting system actually makes matters worse as far as vibration isolation is concerned. When the frequency ratio is greater than √2, it is seen that the transmissibility is smaller than unity and hence, the supporting system functions as a vibration isolator. Damping is seen to be advantages only in the region when the frequency ratio is less than √2 (where a spring mounting supporting system makes matters worse) and not when the frequency ratio is greater than √2 (where a spring mounting supporting system acts as an effective vibration isolator). This is not so important actually as the undesirable effects of high values of damping at frequency ratios greater than √2 is not so great especially at even higher frequency ratios, i.e. achieved by making the supporting system even more flexible. Also, in the unfortunate circumstance that the resonance region of frequency ratio less than √2 is somehow attained; high levels of damping are extremely effective. For good isolation, it is often recommended to design the supporting system for a frequency ratio of at least 3. 384 Structural Engineering Analysis and Design Second Edition Note that the above relationships were based on the absolute terms of acceleration, velocity and displacement, not the relative. The expression for u as depicted in the diagrams is always the absolute displacement. The notion of relative terms only arises when we have support motion. Note that in absolute terms, we need the support displacement and velocity in the equation of motion whilst in relative terms we need only the support acceleration in the equation of motion. Finding an expression for the relative displacement can be useful especially if we want to calculate the shear and bending forces induced in the isolating system. Of course we could subtract the absolute quantities, but this may prove difficult, as the there is a phase difference between the input and response quantities. In absolute terms, the equation of motion m& u&( t ) + c(u&( t ) − u&s ( t ) ) + k (u ( t ) − u s ( t ) ) = 0 In relative terms u r ( t) = u(t ) − u s (t) Hence, m(& u&r ( t ) + & u&s ( t ) ) + cu&r ( t ) + ku r ( t ) = 0 m& u&r ( t ) + cu&r ( t ) + ku r ( t ) = −m& u&s ( t ) Re placing u s ( t ) = u 0 sin ωt m& u&r ( t ) + cu&r ( t ) + ku r ( t ) = mω 2 u 0 sin ωt This equation is similar to that of the harmonic loading except that the harmonic force excitation amplitude is now mω2u0. Hence the steady state solution for the relative displacement is u r (t ) = = mu 0 ω 2 / k (1 − ω 2 ω 2n ) 2 + ( 2ζω / ω n ) 2 u 0 ω / ω 2n 2 (1 − ω 2 ω 2n ) 2 + ( 2ζω / ω n ) 2 sin (ωt − θ ) θ = tan −1 sin (ωt − θ ) 385 2ζω / ω n (1 − ω 2 ω 2n ) θ = tan −1 2ζω / ω n (1 − ω 2 ω 2n ) Structural Engineering Analysis and Design Second Edition 4.6 4.6.1 GL, ML Frequency Domain Analysis – Deterministic and Random Dynamic Response Analysis Mathematical Preliminaries of Representing Dynamic Characteristics in the Frequency Domain The complex frequency response function (FRF) due to a loading {P(ω)} is defined as {F(ω)} = −ω 2 {P(ω)} [M ] + iω[C] + [K ] The complex transfer function (a.k.a. the dynamic flexibility matrix) is defined as the complex frequency response function due to unit harmonic excitations [H(ω)] = 1 − ω [M ] + iω[C] + [K ] 2 This is the so-called transfer function that transfers the excitation to the response as follows [ {u ( t )} = Re al [H(ω)]{P(ω)}e iωt ] The displacement transfer function H(ω) (steady state displacement response per unit harmonic force) is known as the receptance. The velocity transfer function ωH(ω) (steady state velocity response per unit harmonic force) is known as the mobility. The acceleration transfer function ω2H(ω) (steady state acceleration response per unit harmonic force) is known as the inertance. The transfer function or the dynamic flexibility matrix [H(ω)] is actually the Fourier Transform of the unit impulse response matrix [h(t-τ)] (a.k.a. dynamic stiffness matrix) defined for the (implicit) time domain (for modal solutions; not direct solutions). The (magnitude of the) dynamic amplification factor D(ω) is defined as the magnitude of the complex response function {F(ω)} divided by the static displacement. In (implicit) time domain solutions based on modal methods, the unit impulse response matrix (a.k.a. dynamic stiffness matrix) is the crucial matrix that transforms the excitation to the response as described by the Duhamel’s or convolution integral expression as follows {u ( t )} = ∫ [h (t − τ)]{P(τ)}dτ t 0 This impulse response matrix [h(t-τ)] (a.k.a. dynamic stiffness matrix) is actually the Inverse Fourier Transform of the dynamic flexibility matrix or the transfer function [H(ω)] defined for the frequency domain. A unit impulse is theoretically a force time history that occurs over zero time, but has a unit value of the integral of force/time curve. That obviously implies infinite force, which can't exist in reality, but is a very useful approximation when the time of the impulse is short compared to the periods of interest in the response. The response in the time domain to an impulse excitation can be calculated using the Duhamel's Integral (Convolution Integral). A unit impulse excitation will produce what is known as the unit impulse response matrix function (a.k.a. dynamic stiffness) in the time domain. Now, the unit impulse response matrix function (a.k.a. dynamic stiffness) is the Inverse Fourier Transform of the dynamic flexibility matrix (i.e. the transfer function). Conversely, the dynamic flexibility matrix (i.e. the transfer function) is the Fourier Transform of the unit impulse response matrix function (a.k.a. dynamic stiffness). 386 Structural Engineering Analysis and Design Second Edition 4.6.2 GL, ML Vibration Testing The purpose of the vibration testing is to establish the modal properties (modal frequencies, modal mass and modal damping) of the system for correlation with the finite element model. Vibration testing is also used to establish the response to certain excitations to be compared to that of the finite element model to verify the analysis procedure. The vibration test could either be (i) (ii) (iii) Impact (Hammer or Heel-Drop) Test (Artificial Excitation) – For Model Correlation Shaker Table Test (Artificial Excitation) – For Model Correlation Response Measurements (Actual Excitation) – For Analysis Procedure Verification For model correlation, the vibration tests can be used to measure the applied excitation and the structural response. For analysis procedure verification, the vibration test measures the RESPONSE of the structure to the induced excitations, not the actual excitations themselves. 4.6.2.1 Vibration Testing for Model Correlation Vibration Test Impact Test and Logarithmic Decrement Impact Test and Transfer Function FE Equivalent SOL 109 with impact force excitation SOL 109 with impact force excitation Response Time history signal of ensuing free vibration, the frequency content of which can be obtained by FFT. Note that this is NOT the frequency response function FRF, F(ω). The phase information is random. Time history signal of ensuing free vibration and the knowledge of the excitation function can be used to derive unit impulse response matrix (a.k.a. dynamic stiffness matrix), h(tτ) from {u ( t )} = ∫ [h(t − τ)]{P(τ)}dτ t 0 which can transformed by Forward FFT to obtain the complex transfer function H(ω) (a.k.a. the dynamic flexibility matrix) Shaker Table Test and Frequency Response Function SOL 108 with wide-band harmonic excitation Frequency response function FRF, F(ω) Shaker Table Test and Transfer Function SOL 108 with wide-band harmonic excitation Frequency response function FRF, F(ω) which divided by the excitation static force provides the transfer function H(ω) 387 Derived information With knowledge of frequency content, time history signal can be signal processed (i.e. filtered) to yield single mode time history, which by logarithmic decrement provides modal damping H(ω) (with real and imaginary or magnitude and phase info) provides frequency content, modal damping and modal mass. H(ω) (with only magnitude info) provides frequency content and approximate modal damping by half-power bandwidth. F(ω) (with real and imaginary or magnitude and phase info) provides frequency content, modal damping and modal mass. F(ω) (with only magnitude info) provides frequency content and approximate modal damping by half-power bandwidth. H(ω) (with real and imaginary or magnitude and phase info) provides frequency content, modal damping and modal mass. H(ω) (with only magnitude info) provides frequency content and approximate modal damping by half-power bandwidth. Structural Engineering Analysis and Design Second Edition 4.6.2.1.1 Impact Test and Logarithmic Decrement The impact excites the natural modes of vibration. An impact test produces an impulse, which excites the modes, of course some more than others. Response Spectrum 2.5 2 Dimax 1.5 1 0.5 0 0 0.5 1 1.5 2 2.5 3 3.5 4 4.5 td/T i It is really not necessary to know which modes are excited more as we are really only interested in finding out the natural frequencies of the structure, not the response. To perform signal processing of the impact test (I) First, read in all the acceleration time history signals (II) For each acceleration time history signal (i) Plot the signal; ∆t = t2 – t1; sampling frequency = 1/∆t (ii) FFT/PSD (use linear scale instead of logarithmic) the signal to establish its frequency content For each mode of interest (iii) Design a filter to filter the mode of interest for damping estimation. Employ the Butterworth IRR Algorithm, specify the sampling frequency, specify the order and whether it is a low-pass, high-pass or band-pass filter (iv) Filter the signal and plot the (single frequency) filtered signal (v) FFT/PSD the (single frequency) filtered signal to ascertain the effectiveness and accuracy of the filter 388 Structural Engineering Analysis and Design Second Edition (vi) Perform a logarithmic decrement on the (single frequency) filtered signal to determine the modal damping of the mode of interest Next mode of interest Next acceleration time history signal The impact test establishes the natural frequencies and the damping of the structure and is useful for model correlation. Clearly, this method is reliable only if the modes are well spaced out. 389 Structural Engineering Analysis and Design Second Edition 4.6.2.2 Vibrating Testing For Analysis Procedure Verification Response measurements are made to verify the FE analysis procedure. Note that the starting transient occurs at the natural frequencies of the structure whilst the steady-state response is at the frequencies of excitation. To perform signal processing of the response measurements, first read in all the acceleration or velocity time history signals. For each time history (I) Compare the peak of the UNFILTERED time history with established criteria. (II) Compute the (1.0s say) RMS of the ULFILTERED time history. Compare the maximum RMS (of the RMS values from each 1.0s window) with established criteria. Note that the RMS over the entire duration will be lower than over short intervals such as 1.0s. (III) To compare the peak and the (1.0s say) RMS of the FILTERED time history with established criteria, (i) Plot the signal; ∆t = t2 – t1; sampling frequency = 1/∆t. (ii) Design a filter to filter the signal into its 1/3rd octave bands. Employ the Butterworth IRR Algorithm, specify the sampling frequency, specify the order and band-pass filter. (iii) Filter the signal and plot the filtered signals. (iv) (v) Compute the peaks of each 1/3rd octave band filtered signal. Compare the peak values from each 1/3rd octave band filtered signal with established (frequency dependent) criteria. Compute the RMS of each filtered signal in time intervals of 1.0s say. Compute the maximum RMS (of the RMS values from each 1.0s time interval) for one RMS value for each 1/3rd octave band. Note that the RMS over the entire duration will be lower than over short intervals such as 1.0s. Compute the maximum RMS (of the RMS values for each 1/3rd octave band) and compare with established (frequency dependent) criteria. Note also that the unfiltered RMS will be larger than the filtered RMS. Next time history signal 390 Structural Engineering Analysis and Design Second Edition 4.6.3 GL, ML Steady-State Response of Deterministic Periodic (Not Necessarily Harmonic) Long Duration Excitation Utilizing Fourier Series (or Generally Utilizing Fast Fourier Transforms FFT) The solution method can be used to solve dynamic systems subjected to: (a) Deterministic periodic non-harmonic long duration loading functions In this LINEAR FREQUENCY DOMAIN solution, not only that the static response has to be added separately, but also the mean of the dynamic excitation has also got to be added separately as a static response. This is because the mean of the dynamically applied force is not included in the dynamic excitations. Hence the total response in this frequency domain dynamic analysis = static response to mean of dynamic excitation + dynamic response + static response to static loads. 4.6.3.1 Fourier Series The French Mathematician J. Fourier (1768-1830) postulated that any deterministic periodic function can be expressed as the summation of a number of sinusoidal waves of varying frequency, amplitude and phase. A deterministic periodic (of period T) function that is not necessarily harmonic can thus be expressed as a summation of an infinite number of sine and cosine terms, i.e. a Fourier Series. Forced responses (steady-state) are performed in the frequency domain with these individual harmonics (with the correct amplitudes and phase differences) as the excitations. Note that since this method is performed in the frequency domain, the response calculated is the steady-state response. Hence, it is assumed that the excitation is periodic and long enough for steady-state conditions to be achieved. The total steady-state response is thus the summation of the responses of the individual harmonics. A general deterministic periodic (of period T) function that is not necessarily harmonic can be expressed as a summation of an infinite number of sine and cosine terms, i.e. a Continuous Fourier Series. P( t ) = a 0 + ∞ ∑ [a n cos nωt + b n sin nωt ] n =1 1 T 2 T 2 T P( t )dt a n = P( t ) cos nωtdt b n = P( t ) sin nωtdt T 0 T 0 T 0 The constant a0 is the mean component of the force. The coefficients an and bn which is constant for each harmonic n, is the amplitudes of the harmonics. Usually only the first few harmonics need to be included as the response to higher harmonics may be negligible. An illustration is presented for a saw tooth function. a0 = ∫ ∫ ∫ The Fourier Series representation is as follows. Even with only 3 Fourier terms, the representation is pretty good. 391 Structural Engineering Analysis and Design Second Edition The total response will then be the summation of all the responses due to the individual harmonics. For a SDOF system, the steady-state response due to the constant a0 force is u mean ( t ) = a0 k The steady-state response due to a ancosnωt force u cos ( t ) = ( ) (1 − nω 2 an / k ω 2n ) 2 + (2ζnω / ω n ) cos( nωt − θ) θ = tan −1 2 2ζnω / ω n ( ) (1 − nω 2 ω 2n ) The steady-state response due to a bnsinnωt force u sin ( t ) = ( ) (1 − nω 2 bn / k ω 2n ) 2 + (2ζnω / ω n ) 2 sin( nωt − θ) θ = tan −1 2ζ nω / ω n ( ) (1 − nω 2 ω 2n ) The total SDOF steady-state response is thus the summation of the above three components for all harmonics m. u ( t ) = u mean (t ) + ∞ ∑ [u cos ( t ) + u sin ( t )] n =1 4.6.3.2 Discrete Fourier Series In the Fourier Series Analysis, the original continuous loading function P(t) can be represented exactly by a continuous function if an infinite (Fourier) series is adopted. Now, if the function P(t) is supplied only at N equally spaced time intervals (∆t = T/N) t0, t1, t2, … ,tN-1, where tj = j∆t, the Discrete Fourier Series results P( t j ) = a 0 + ∞ ∑ [a n cos nωt j + b n sin nωt j ] n =1 a0 = an = bn = 1 T N −1 ∑ P( t j) j= 0 N −1 2 T ∑ P( t 2 T ∑ P( t j ) cos nωt j ∆t j= 0 N −1 j ) sin nωt j ∆t j= 0 392 Structural Engineering Analysis and Design Second Edition Whereas the Fourier Series could represent a deterministic continuous and periodic function exactly if an infinite number of harmonics were utilized, the Discrete Fourier Series can represent a deterministic discrete and non-periodic function exactly only at the discrete points if an infinite number of harmonics are adopted. 4.6.3.3 Discrete Fourier Series in Complex Notation In practice the Fourier coefficients a0, an and bn prove very cumbersome to manipulate algebraically. Complex number theory helps with this aspect as all three coefficients may be replaced by one complex coefficient Cn. Recapping basic complex number theory, a complex number contains real and imaginary components z = x + iy it can be written in a polar form by computing the magnitude and the phase z =  x 2 + y 2  z =  x 2 + y 2  e iθ , θ = tan −1 ( y / x )  (cos θ + i sin θ), θ = tan −1 ( y / x )  Writing [a n cos nωt + b n sin nωt ] = Re al[a n cos nωt + ia n sin nωt − ib n cos nωt − i 2 b n sin nωt ] = Re al[(a n − ib n )(cos nωt + i sin nωt )] [ = Re al Λ n e inωt ] the Discrete Fourier Series can be rewritten in complex notation as follows ∞ inωt  P( t j ) = a 0 + Re al  Λ n e j   n =1  Λ n = a n − ib n ∑ but since an = 2 T N −1 ∑ P( t ) cos nωt ∆t j j and bn = j= 0 2 T N −1 ∑ P(t ) sin nωt ∆t j j j= 0 we have Λ n = a n − ib n = 2 T N −1 ∑ P( t j )e − inωt j ∆t j= 0 and thus the Discrete Fourier Series can be rewritten in complex notation as follows ∞ inωt  P( t j ) = a 0 + Re al Λ n e j   n =1  ∑ Λn = 2 T N −1 ∑ P( t j )e −inωt j ∆t j= 0 393 Structural Engineering Analysis and Design Second Edition 4.6.3.4 Double Sided Discrete Fourier Series in Complex Notation The Discrete Fourier Series in Complex Notation expression may be simplified even further by the introduction of negative frequencies. These have the effect of cancelling the imaginary components and hence allowing the Real[…]function to be dropped as presented below. 1 2 P( t j ) = a 0 + Λn = 2 T ∞ ∑ Λne inωt j + n =1 N −1 ∑ P( t j )e −inωt j 1 −∞ inωt Λne j 2 n = −1 ∑ ∆t j= 0 To prove that the Double Sided expression is the same as the single sided with Re […] expression, the following back analysis is performed. 1 2 P( t j ) = a 0 + 1 2 = a0 + 1 2 = a0 + 1 2 = a0 + = a0 + ∞ ∑ Λne inωt j + n =1 1 −∞ inωt Λne j 2 n = −1 ∑ ∞ −∞ 1 ∑ (a n − ib n )(cos nωt j + i sin nωt j ) + ∑ (a n 2 n = −1 n =1 ∞ ( − ib n ) cos nωt j + i sin nωt j ) ∞ 1 ∑ (a n − ib n )(cos nωt j + i sin nωt j ) + ∑ (a n + ib n )(cos nωt j − i sin nωt j ); Note Λ −n = a n + ib n 2 n =1 ∞ ∑ (2a cos nωt j + 2b n sin nωt j n n =1 ) n =1 ∞ ∑ (a n cos nωt j + b n sin nωt j ) n =1 ∞ inωt  = a 0 + Re al Λ n e j   n =1  ∑ Hence, proven. We then change the limits of the summation the Fourier coefficients so that a0 and Λn can be replaced with the single complex Fourier coefficient Cn. Hence from P( t j ) = a 0 + Λn = 2 T 1 2 ∞ ∑ Λne inωt j + n =1 N −1 ∑ P( t j )e −inωt j 1 −∞ inωt Λne j 2 n = −1 ∑ ∆t j= 0 we thus have P( t j ) = ∞ ∑C ne inωt j n = −∞ Cn = 1 1 Λn = 2 T N −1 ∑ P( t j )e − inωt j ∆t j= 0 where even the a0 term is accounted for by Cn. Knowing that tj = j∆t, T = N∆t and ω = 2π/T P( t j ) = ∞ ∑C ne 2 πi ( nj / N ) n = −∞ Cn = 1 N N −1 ∑ P( t j )e − 2 πi ( nj / N ) j= 0 394 Structural Engineering Analysis and Design Second Edition Hence we have derived the Double Sided Discrete Fourier Series in Complex Notation. This expression is is said to be double sided because it uses both positive and negative frequencies to represent the Fourier coefficients. From the Double Sided Discrete Fourier Series in Complex Notation, we now define the Discrete Fourier Transform of the series P(tj) as Cn. Cn = 1 N −1 P ( t j )e − 2 πi ( nj / N ) N j= 0 ∑ Because the phase information is also stored, the time signal can be regenerated from the Discrete Fourier Transform using the Discrete Inverse Fourier Transform P( t j ) = ∞ ∑C e 2 πi ( nj / N ) n n = −∞ Whereas the Fourier Series could represent a deterministic continuous and periodic function exactly if an infinite number of harmonics were utilized, the Double Sided Discrete Fourier Series in Complex Notations can represent a deterministic discrete and non-periodic function exactly only at the discrete points if an infinite number of harmonics are adopted. 4.6.3.5 Normalized Double Sided Discrete Fourier Series in Complex Notation Each Fourier coefficient Cn is obtained for a frequency of n/T Hz, the frequency interval between each coefficient ∆f is therefore 1/T Hz. This causes problems as the frequency at which the coefficients are calculated is dependent on the period T chosen. It is common practice to normalize the Fourier Transform coefficients Cn to eliminate the dependence on T. The normalized coefficients take the form of a density function and the Fourier coefficient is obtained from the area under the density curve for the range ∆f = 1/T in question. The Inverse Fourier Transform is thus ∞ 1 ∞ Note that here T is instead of P( t j ) = c n e 2 πi ( nj / N ) P( t j ) = C n e 2 πi ( nj / N ) T n = −∞ period, not duration! n = −∞ ∑ ∑ and the Fourier Transform Density Function is cn = T N −1 P( t j )e − 2 πi ( nj / N ) instead of N j= 0 ∑ Cn = 1 N −1 P ( t j )e − 2 πi ( nj / N ) N j= 0 ∑ The Fourier Transform Density Function and Inverse Fourier Transform transformations are illustrated. 395 Structural Engineering Analysis and Design Second Edition Whereas the Fourier Series could represent a deterministic continuous and periodic function exactly if an infinite number of harmonics were utilized, the Normalized Double Sided Discrete Fourier Series in Complex Notations can represent a deterministic discrete and non-periodic function exactly only at the discrete points if an infinite number of harmonics are adopted. With the definition of the Fourier Density Function, the amplitude and phase of a frequency component with frequency f is now obtained by taking the magnitude and argument of the sum of area under the density curve within ∆f at f and -f. The area under the Fourier Density Function is given as a complex number; the amplitude content can be obtained by taking the modulus of this complex area and the phase content from the argument or this complex area. The Fourier Density Function of a stationary random signal is a plot of amplitude (and phase) against frequency. A sine wave of frequency ω, amplitude A and initial phase angle φ is represented in the frequency domain by a spike occurring at ω along the frequency axis. If the magnitude of the complex Fourier Density Function is plotted, then the area under the spike is found to be the amplitude A of the sine wave. When the argument of the complex Fourier Density Function is plotted then the area is found to be initial phase angle φ of the sine wave. Therefore, if we want to find the amplitude and phase of the sinusoidal waves in a particular frequency range, say between 2 and 2.5 Hz, we can measure the area under the curve in that frequency range. 4.6.3.6 Symmetrical Normalized Double Sided Discrete Fourier Series in Complex Notation In order to maintain the symmetry with its transform pair, i.e. the Discrete Fourier Transform Density Function cn = T N −1 P( t j )e − 2 πi ( nj / N ) N j= 0 ∑ the Discrete Inverse Fourier Transform is limited to only N terms (i.e. from 0 to N–1) as follows P( t j ) = 1 N −1 c n e 2 πi ( nj / N ) T n =0 ∑ It is paramount to realize that in the Discrete Inverse Fourier Transform summation indicated above, the frequencies increase up to only N/2 and not N−1. This is because it can be shown that for n > N/2, the 396 Structural Engineering Analysis and Design Second Edition corresponding frequencies are equal to the negative frequencies of order N−n. This fact restricts the harmonic frequency components that may be represented in the series to a maximum of N/2. The frequency corresponding to this maximum order ωN/2 = (N/2)ω is known as the Nyquist frequency (a.k.a. folding frequency). Moreover, if there are harmonic components above ωN/2 in the original function, these higher components will introduce distortions in the lower harmonic components of the series, a phenomenon known as aliasing. Hence, it is recommended that the number of sampled points, N should be at least twice the highest harmonic component present in the function. Whereas the Fourier Series could represent a deterministic continuous and periodic function exactly if an infinite number of harmonics were utilized, the Symmetrical Normalized Double Sided Discrete Fourier Series in Complex Notations can represent a deterministic discrete and non-periodic function approximately only at the discrete points since the number of harmonics is limited to N/2 i.e. from -N/2 to N/2 instead of ∞ i.e. from –∞ to ∞ and if components of frequency higher than the Nyquist, ωN/2 = (N/2)ω = (N/2)(2π/T) = πN/T = π/∆t exist in the time signal, aliasing (distortions in the lower harmonic components) occurs, noting however that the latter reason is user avoidable. 4.6.3.7 Symmetrical Normalized Single Sided Discrete Fourier Series in Complex Notation The Single Sided Fourier Transform Density Function contains the same information as the Double Sided Fourier Transform Density Function but is often more convenient to use as negative frequencies are not considered. In order to maintain the same intensity of the original time signal, the Single Sided Fourier Transform Density Function is doubled. The Single Sided Discrete Fourier Transform Density Function of the series P(tj) and the corresponding Single Sided Discrete Inverse Fourier Transform are respectively cn = 2T N / 2 P( t j )e − 2 πi ( nj / N ) N j= 0 ∑ and P( t j ) = 1 T N −1 ∑c ne 2 πi ( nj / N ) n =0 The following time history will produce the following Double Sided Fourier Transform Density Functions. And the time history will instead produce the following Single Sided Fourier Transform Density Functions. 397 Structural Engineering Analysis and Design Second Edition 4.6.3.8 Practicalities of the Specification of the Fast Fourier Transform (FFT) Representation An extremely efficient computational algorithm, which employs the Discrete Fourier Transform concept is the Fast Fourier Transform (FFT). Note that whereas the Fourier Series can represent deterministic periodic functions, the Fast Fourier Transform FFT can represent deterministic non-periodic functions. Again, since the FFT method is performed in the frequency domain, the response calculated is the steady-state response. Hence, it is assumed that the excitation is periodic and long enough for steady-state conditions to be achieved. The concept of Fourier Series and the Fast Fourier Transform representations is presented. Fourier Series Method Represents Deterministic, Periodic Functions Fast Fourier Transform Method Represents Deterministic, Non-periodic Functions However, since the analysis is performed in the frequency domain, the response is steady-state and hence we shall use the Fast Fourier Transform FFT method to solve excitations which are deterministic, periodic and long duration for steady-state conditions to be achieved. Hence, forced response due to an impulse must be performed in the time domain and cannot be performed in the frequency domain although h(t−τ) and H(ω) are a Fourier Transform pair. This means that although the excitation in the time and frequency domains and the structural characteristics (h(t−τ) and H(ω)) are interchangeable with the Fourier Transforms, the response in the time and frequency domain are only comparable if the excitation is deterministic, periodic and long duration for steady state conditions to be achieved, a condition which is not achieved for an impulsive excitation. The FFT must follow certain rules. The time signal should follow the 2N rule, N an integer. This means that the number of data points within the time signal should be 32, 64, 128, 256, 512, 1024, 2048 … 131072 for the FFT to be computed. Three considerations should be made in choosing the parameters digitizing a time history signal. Firstly, if N is the number of sample intervals, it can be shown mathematically that the Discrete Inverse Fourier Transform representation is restricted to a maximum of N/2 harmonic components in the series, i.e. N/2 spectral lines. Number of points in positive FFT = 1 x number of points in time signal, N 2 This occurs because for n > N/2, the corresponding frequencies are equal to the negative of frequencies order N-n. Secondly, the maximum harmonic component that can be represented is (N/2)ω, where ω here is 2π/T, T being the entire duration of loading. N N 2π N 2π π ω= = = 2 2 T 2 N∆t ∆t ωy 1 fy = = 2π 2∆t ωy = In other words, 1 x sampling frequency 2 1 1 = x 2 time step, ∆t Nyquist Frequency, f y = The frequency of this maximum harmonic component is called the Nyquist frequency or the folding frequency. Thirdly, if harmonic components above the Nyquist frequency were present in the original function, it would introduce distortions in the lower harmonic components of the series, a phenomenon called aliasing. The sampling frequency must then be two times the highest frequency component so that the Nyquist frequency (which is half the sampling frequency) becomes equal to the highest frequency component of interest. This is also obvious from observation of the function. A triangular pulse of a frequency of 100Hz 398 Structural Engineering Analysis and Design Second Edition (period 0.01s) requires at least 3 sampling points to define the triangular shape. Three sampling points here means that the sampling frequency will be 200Hz (0.005s). The Nyquist frequency will then be 200Hz/2 = 100Hz, which again is the frequency of that of the triangular pulse. Hence the FFT should represent all the frequency components of the original time signal to avoid aliasing. USER CHOICE (CHOOSE 2 OF 4) CONSEQUENCE Nyquist Number ∆f = Nyquist Time Sampling Number Frequency = of Frequency / Duration Step, Frequency of Time Sampling Spectral Number of = N∆t (s) Frequency / Lines = Spectral Lines ∆t (s) = 1/∆t (Hz) Steps, N 2 (Hz) N/2 (Hz) 0.02 0.02 0.04 0.01 50 50 25 100 1024 2048 1024 1024 20.48 40.96 40.96 10.24 25 25 12.5 50 512 1024 512 512 0.049 0.024 0.024 0.098 Remark Original More resolution More resolution, lower Nyquist Less resolution, higher Nyquist We can make a couple of conclusions. First, the time step should be chosen to capture all frequency components of the time signal so that the Nyquist frequency (which is half the sampling frequency) is at least equal to the highest frequency component to avoid aliasing. To be sure of this, one may filter the signal electronically to remove all frequencies above the Nyquist frequency. Second, the more the number of time steps, N and/or the larger the time step ∆t (so long as the sampling frequency 1/∆t is still at least twice the highest frequency component in the time signal to avoid aliasing) the better the resolution as ∆f = 1/T. Hence, for example, if say we are interested in capturing a time signal with frequency components up to say 25Hz, we thus specify a digitizing sampling frequency of 50Hz (so that the Nyquist frequency which is half the sampling frequency equals the highest frequency of interest) i.e. a time step of 0.02s whilst filtering all frequencies above 25Hz to avoid aliasing. Then, we choose the number of time steps, N of 1024, 2048, 4096 etc … and hence the duration N∆t so that an acceptable resolution is obtained on the Fourier Transform Density Function knowing that the number of spectral lines is N/2. 399 Structural Engineering Analysis and Design Second Edition 4.6.3.9 MSC.NASTRAN Fast Fourier Transform Analysis Methodology The Fourier Transform method provides an efficient alternative method of determining the steady-state transient response of the equations of motion. It avoids the lengthy time integration of the transient equations of motion with the repetitive periodic input of the loading function. Time-dependent applied loads are transformed to the frequency domain using the Double Sided Fourier Transform Density Function cn = T N −1 P( t j )e − 2 πi ( nj / N ) N j= 0 ∑ before all frequency dependent matrix calculations are completed in the frequency domain. {u (ω n )} = [H (ω)]{c n } Then using the Inverse Fourier Transform P( t j ) = 1 T N −1 ∑ u (ω n )e 2 πi ( nj / N ) n =0 the frequency response solution variables are then transformed back into the time domain. The steady-state response to the forcing function P(tj) is thus [ {u ( t j )} = Re al [H (ω)]P( t j ) 1 = Re al  T ] c n e 2 πi ( nj / N ) N −1  ∑ − ω [M] + iω[C] + [K]  n =0 2 Fourier transform methods have been implemented in MSC.NASTRAN to integrate the equations of motion in order to obtain the aeroelastic response of fixed wing aircraft. This capability is especially important for this type of analysis since the unsteady aerodynamic matrices are known only in the frequency domain. The Fourier transform method may also be used to solve for the transient response of conventional structural models (no aerodynamic effects) subjected to periodic loads. This capability is available in SOL 108 and SOL 111 for frequency response output data. For transient type output, SOL 146 must be used. The transformation is performed quite simply when the requested load is the time dependent TLOADi form instead of a frequency dependent RLOADi entry. In MSC.NASTRAN, two forms of the Fourier transform are available, namely the Fourier series and the Fourier integral. Both methods require necessary numerical compromises and hence produce numerical approximations. In the Fourier series, the basic time interval is 0 < t < T, with the function periodic. The circular frequencies are given by where T is a large time equal to the period of the lowest forcing frequency. The load transformation for a load at point a is given for each requested frequency by The response at point j is given by 400 Structural Engineering Analysis and Design Second Edition where Hja(ωn) is the frequency response of any physical variable due to unit load. The response in the time domain is given by In the Fourier Integral, the time interval is the limit as T ∞, ∆f 0, and 2πn∆f ω of the Fourier series. Here, ω is a continuous variable. The corresponding load transformation, frequency response and time domain response relationships are presented. The approach that must be undertaken by the user in MSC.NASTRAN is described. (a) The solution scheme must be SOL 108, SOL 111 or SOL 145. The SOL 145 requires the cards of SOL 111 with the addition of TSTEP Case Control and Bulk Data cards. (b) The user must define a time domain function that vanishes for t > T. Note that T is the interval of the periodic function. For piecewise linear tabular functions (TLOAD1), a table of pairs (xi, Yi)(i = 1,N) prescribes N-1 time intervals. If an X1 shift and an X2 scale factor are included, the time-dependent load at point a is given by where Aa is an amplitude factor and τa is a delay factor that may depend upon the loading point. Likewise, the general function (TLOAD2) is defined by The value of n must be an integer for transient analysis by the Fourier method. Do not mix loading functions of RLOADi with TLOADi. (c) Use constant frequency spacing, ∆f = 1/T (d) Three approximation methods are available to evaluate the inverse Fourier transform which may be selected by the user via the parameter IFTM, namely Method 0, Method 1 and Method 2. Consider the response of a simple damped oscillator to a pulse. The upper three curves show the pulse and the response of the system if it is very stable and slightly stable. Using the Fourier method, the pulse is replaced by a series of pulses, with period . 401 Structural Engineering Analysis and Design Second Edition As can be seen, this method gives good results if the system is damped, but an incorrect impression if the system is lightly damped. Thus, in order for the results of the Fourier method to be valid: 1. The system should be reasonably well damped. 2. The forcing function should be zero for some time interval to allow decay. 3. The frequency interval In general, Methods 1 and 2 are more accurate than Method 0. However, these methods introduce positive artificial damping into the result that may lead to erroneous conclusions in stability studies. Note that an alternative to the Fourier Method is to perform a SOL 108 or SOL 111 with multiple RLOADi entries to define the different harmonics of the signal, with the correct phase difference. This of course depends on knowing the harmonics which could be derived by manually performing an FFT on the periodic signal. 402 Structural Engineering Analysis and Design Second Edition 4.6.4 GL, ML Steady-State Response of Random, Gaussian, and Stationary (and Ergodic) Excitations Utilizing Power Spectral Density (PSD) Functions The solution method can be used to solve dynamic systems subjected to: (a) Random stationary (and ergodic) long duration loading functions In this LINEAR FREQUENCY DOMAIN solution, not only that the static response has to be added separately, but also the mean of the dynamic excitation has also got to be added separately as a static response. This is because the mean of the dynamically applied force is not included in the dynamic excitations. Hence the total response in this frequency domain dynamic analysis = static response to mean of dynamic excitation + dynamic response + static response to static loads. 4.6.4.1 Statistic of Time Domain Function The statistics of a random function P(t) of duration T can be characterized by (a) The mean, which is usually zero P= (b) 1 T P( t )dt T o ∫ The root mean square (RMS) and root mean quad (RMQ), the latter gives greater weight to higher values 1/ 4 1 T 2 1 T 4  P ( t )dt RMQ =  P ( t )dt  o T o T   Note that the RMS of a continuous simple harmonic motion is amplitude/√2. ∫ RMS = (c) The standard deviation, which is equal to the RMS when the mean is zero σ= (d) ∫ 1 T ∫ [P(t) − P] dt = (RMS) − (P ) T 2 2 2 o The Gaussian (a.k.a. normal) probability density function PDF to define the amplitude of the (narrowband and broadband) random function P(t). The area under the PDF defines the probability of occurrence. Random loading functions P(t) usually follow the Gaussian (or normal) PDF distribution which is a function of the mean and the standard deviation. The Gaussian is bell-shaped and is symmetrical about the mean. Gaussian Pr obability(P1 ≤ P ≤ P2 ) = ∫ P2 PDF(P)dP P1 1 2 πσ ∫ = P2 P1 e − ( ) 1 2 P− P / σ2 2 dP On integration of the Gaussian, it is shown that, the probability of P lying within 1 standard deviation from the mean is 68.3%, within 2 standard deviations is 95.4% and within 3 standard deviations is 99.7%. (e) The Rayleigh distribution to define the peaks A of the (narrowband) random vibration functions P(t). The Rayleigh distribution is a function of the standard deviation. Rayleigh Pr obability(A1 ≤ A ≤ A 2 ) = ∫ A2 = ∫ A2 A1 PDF(A)dA A1 403 A − A 2 / 2σ 2 e dA, σ2 A>0 Structural Engineering Analysis and Design Second Edition The best way to visualize the amplitude and peak PDFs is to draw tram lines horizontally through the time history and then count either the number of times the signal crosses the tram lines or the number of times a peak occurs in-between the tram lines. The complete PDFs are obtained by repeating this process for all horizontal levels in the signal. (f) The irregularity factor characterizing the frequency content and bandedness of the time signal P(t) in the time domain. The irregularity factor is defined as Irregularity factor, γ = E[0] ; 0 < γ <1 E[P] where E(0) is the expected number of upward mean crossings and E(P) is the expected number of peaks. Note that γ = 0.0 indicates white noise and γ = 1.0 indicates a pure sine wave. Practical values are presented. γ = 1.0 Sine wave γ ≈ 1.0 Narrowband process γ ≈ 0.7 to 0.95 Broadband process γ < 0.7 White noise process A narrowband process is typically recognized in the time history by the amplitude modulation, often referred to as a beat envelope. An important observation made of narrowband processes is that the peak and trough of the time signal amplitude envelope is symmetrical about the time axis. This occurs because the frequency content is in a narrowband and is thus almost similar to each other, and so the time signal always passes through the mean (zero amplitude usually) in every cycle. It is interesting to note that the amplitude probability density function (PDF) of a narrowband signal is Gaussian whilst the peak PDF is Rayleigh in distribution. The time signal of a broadband process is not symmetrical about the time axis. This occurs 404 Structural Engineering Analysis and Design Second Edition because the frequency content is in a broadband and is thus dissimilar to each other, and so the time signal will not pass through the mean (zero amplitude usually) in every cycle. Hence, a broadband process is typically characterized in the time domain by its positive valleys and negative peaks. It is interesting to note that the amplitude PDF of a wide band signal is Gaussian. (g) The auto-covariance (a.k.a. auto-correlation) characterizing the bandedness of the time signal P(t) in the time domain. The auto-covariance function is defined The notation Cyy indicates the auto-covariance function for a single process y. The notation is introduced to distinguish between the 'cross-covariance function (Cxy)' for two random processes x and y defined as follows. For a zero mean time history, the auto-covariance can be rewritten as the infinite time average as follows. A wide-banded process loses similarity within a short time shift and hence the auto-correlation function becomes zero quickly. A narrowbanded process does not lose similarity and hence it takes a long time for the auto-correlation function to become zero. For periodic processes with period T, the auto-covariance function is also periodic with the same period. For stationary processes the auto-covariance function is even, i.e.Cyy(τ) = Cyy(-τ), and may be expressed as a single sided function. 405 Structural Engineering Analysis and Design Second Edition It is often convenient to normalize the covariance function in order to compare different time histories with different scales of measurement. This is achieved by dividing the covariance by the variance. The normalized covariance function is defined below, it has the same shape as the covariance function except that the ordinate is scaled to have a value of 1 for τ=0. The time scale is defined as the area under the normalized covariance function as below. For a random time history this roughly equates to the mean zero crossing period of the time history. For a periodic time history this is not the case however as . Ty → 0. (h) The cross-covariance function characterizing the correlation between two time signals. We are interested in the sequential relationship between the two time histories. The figure shows two anemometers measuring wind speed placed side by side with separation d. From each anemometer a time history of the wind speed is produced. If the two anemometers are far enough apart then the wind speed witnessed by one will be completely independent of the other, they are said to be uncorrelated. As they are moved closer together then a correlation between the two time histories will be noted. Correlation occurs because the random turbulent wind incident on anemometer x is sufficiently large to also be influencing anemometer y. The covariance function may be used to find the sequential relationships between the two time histories. The notation Cyx is used to describe the cross-covariance function between the two random processes x and y. It effectively tells us what the effect on y would be should a random process hit x. 406 Structural Engineering Analysis and Design Second Edition 4.6.4.2 Definition of the Power Spectral Density (PSD) A random stationary forcing function has an imprecisely known magnitude, however all samples of the forcing function have the same statistical characteristics. The statistics of stationary and ergodic processes can be described by one sample that is sufficiently long in duration. The PSD represents the random function. Consider the transformation from a single sided Fourier Density Spectra (as described in Section 4.6.3.7) to a single sided PSD. The mean amplitude of the component sinusoidal waves over a frequency range ∆f is obtained from the Fourier spectra by taking the modulus of the area under the curve expressed as follows. Amplitude(fn) = ∆f.cn(fn) The area under a PSD represents the mean squared amplitude of the component sinusoidal waves where MeanSquare(fn) = ½[Amplitude(fn)]2. We can equate the mean square amplitudes calculated from the PSD and the Fourier spectra and hence determine the transformation between the two, as follows. 1 2 ∆f .G (f n ) = .∆f 2 . c n (f n ) 2 1 2 ∴ G (f n ) = . c n (f n ) 2.T Note that here T is period, not duration! The transformation from a double sided Fourier Density Spectra (as described in Section 4.6.3.6) to a double sided PSD is expressed as follows. S(f n ) = 1 2 . c n (f n ) T The PSD discards the initial phase information (of the individual harmonic components) of the FFT storing only the amplitude squared and corresponding frequency information. The PSD is hence the modulus squared of the FFT. Because there is no phase information, the PSD is no longer complex unlike the FFT. PSDs are given in many of the design standards where random loading is involved. If the designer wishes to determine how a non-linear structure will react to a typical random load history it is necessary to regenerate a characteristic time history from the design PSD, this can then be analyzed using a dynamic analysis program in the time domain. The PSD contains information on the amplitude and frequency content of the sinusoidal waves but does not show the phase relationships. The discarding of the phase information means that the original signal cannot be reproduced exactly deterministically. However, a random phase description can be applied (using the Inverse Fourier Transform) in order to recreate a signal that is statistically similar. Hence, this means that the creation of a PSD from a time signal should assume that the original signal is random in the first place. 407 Structural Engineering Analysis and Design Second Edition In the past, the time signal used to be transformed to the auto-covariance function, then subsequently into the PSD. Now, with the arrival of the Fast Fourier Transform FFT, the PSD is generated directly from the time signal. The auto- and cross-spectral density functions are defined from the auto- and cross-covariance functions using the Fourier Transform are follows. In fact, the Fourier transform pair can be used to transform between the covariance functions and the PSDs. The auto-covariance function is similar to a time history representation of the PSD. In effect it is the time history of the mean square amplitude of the sinusoidal waves with a zero phase angle. The correlation between two random processes can be described using the coherence function. The coherence represents the degree of correlation between two random processes. Two uncorrelated events show zero coherence where as two fully correlated events show unit coherence. The coherence function is defined below as a ratio of the cross-power spectral density function to the geometric mean of the two auto-power spectral density functions. Many design standards quote the auto-power spectral density function which the designer should use to verify the design. Where there are correlated multiple events it is often easier to express the correlation in terms of the coherence function than to specify many cross-power spectral density functions separately. The designer may then derive his own cross-spectral density functions by rearranging the above equation. For certain analyses, such as wind turbulence, the coherence function is expressed as a function of frequency and separation distance. The regeneration of a time history from the double sided PSD is as follows (noting that y(fn) is another notation for c(fn). 408 Structural Engineering Analysis and Design Second Edition The regeneration of a time history from the single sided PSD is as follows (noting that y(fn) is another notation for c(fn). Practical ball park PSD vibration levels are presented. A PSD of 0.001 g2/Hz over 25 to 250 Hz would be experienced inside a civil airliner. A PSD of 0.01 g2/Hz would be the level most electronic equipment is tested. A PSD of 0.1 g2/Hz would make one feel quite uncomfortable and is typical in military vehicles. A PSD of 1.0 g2/Hz would certainly make one extremely uncomfortable. 409 Structural Engineering Analysis and Design Second Edition 4.6.4.3 Validity of the PSD Representation The specification of a PSD in place of a time signal (for a frequency domain analysis) is valid only when: (i) The signal is random (narrowband or broadband) in phase, i.e. the initial phase between the different harmonic components is random. This may not be always true, in which case the signal is deterministic, and the analysis should thus be performed using deterministic methods in the time or frequency domain. If the time signal has a discernible spike or a superimposed dominating sine wave, then it is unlikely that that will be random. Performing a frequency domain random analysis on a deterministic signal is conservative. For instance, the PSD of a sine wave with an amplitude of say 140MPa is simply a spike. We know that the RMS of the sinusoidal time signal is 0.7071 times the amplitude, hence 100MPa. This RMS will be represented by the square root of the area under the PSD. We also know that generating a random time signal from a PSD will predict a peak amplitude of 3 (to 4.5) times the RMS, hence 300MPa here. This is because the amplitude distribution of a narrow or broadband signal is Gaussian. This is much higher than the 140MPa value of the original signal. Thus the frequency domain approach will be conservative. (ii) The signal is Gaussian in its amplitude probability distribution. This is usually the case. Gaussian means that the peak and amplitude probability density function are gaussian in nature or follow a bell shaped curve as shown here. If you draw tram lines through a signal and count the number of times the signal passes through it and plot that as a density function it is gaussian if it follows a bell shape. An example of a non- gaussian signal is a pure sine wave. However adding multiple sine wave together quickly becomes gaussian. (iii) The signal is statistically stationary (and ergodic). This means that the statistics of the signal does not change with time. This is usually the case. This ensures that the time signal is long enough to be represented by the PSD. Stationarity refers to the fact that the average of the instantaneous displacements of an ensemble of time history samples at a particular arbitrary time ti is the same as the average at any other time ti. In addition, if the average obtained with respect to time for any time history sample within the ensemble of time histories is equal to the average across the ensemble at an arbitrary time ti, the random process is called ergodic. Thus in a stationary, ergodic process, a single record may be used to obtain the statistical description of the random function. 410 Structural Engineering Analysis and Design Second Edition 4.6.4.4 Generation and Specification of the PSD The following aspects are considered in the generation of a PSD from a time signal: (i) (ii) (iii) (iv) (v) (vi) (vii) The number of points in the PSD, NFFT = number of data points / 2 Employ the Welsh Method Employ the Hanning Window. The Hanning window shape accounts for the fact that the signals within the buffers are not periodic, i.e. that they do not start and end at the zero. Incomplete cycles cause spectral leakage, which gives errors in the PSD frequencies and amplitudes. This arises because of Fourier’s assumption that the time history is periodic. Spectral leakage tends to occur with rectangular window functions. The size of the buffer or window, NWIND ( The specification of a PSD should be supplemented with: (i) The mean of the time signal as a PSD does not contain information about the mean A good method to check whether a PSD has been specified correctly from a time signal is to convert the PSD back into a time signal and comparing the statistics of the new signal to that of the original signal. 411 Structural Engineering Analysis and Design Second Edition 4.6.4.5 Statistical Information Provided by the PSD The PSD provides the following information: (i) A description of the frequency content within the signal. The PSD of a constant amplitude sine wave is an infinite amplitude spike. The sine wave cannot be reproduced, as it is not random. A sinusoidal time history appears as a single spike on the PSD plot. The spike is centered at the frequency of the sine wave and the area of the spike represents the mean square amplitude of the wave. In theory this spike should be infinitely tall and infinity narrow for a pure sine wave, however because of the numerical analysis the spike will have a finite width and will therefore have a finite height. Remember, with PSD plots we are interested in the area under the graph and not the height of the graph. The PSD of a narrowband process is a finite amplitude spike within a narrow frequency band. The regenerated amplitude envelope of the time signal will be irregular, but the signal will consist of only a few dominant frequencies. The PSD of a broadband process is a multitude of finite amplitude spikes within a broad frequency band. The PSD of a white noise is flat, i.e. the frequency content of the signal shows a similar weighting to all frequencies. 412 Structural Engineering Analysis and Design Second Edition To quantitatively describe the frequency content or bandedness of the PSD, the irregularity factor, γ can be calculated based on the moments of the PSD. The nth moment of the PSD is Hence, the irregularity factor is defined as follows Irregularity factor, γ = E[0] ; 0 < γ <1 E[P] Expected number of zero crossings, E[0] = Expected number of peaks, E[P] = m2 m0 m4 m2 In theory all possible moments are required to fully characterize the original process. However, in practice we find that m0, m1, m2, and m4 are sufficient. With higher moments of a PSD, greater weighting is given to higher frequencies. The number of zero crossings E[0] is usually the number of mean crossings as the mean is non-existent in the PSD. (ii) The bandedness can be described using the auto-covariance functions which is defined using the Inverse Fourier Transform of the auto-spectral density (PSD). (iii) The correlation between two random processes can be described using the cross-covariance functions which is defined using the Inverse Fourier Transform of the cross-spectral densities (CPSD). 413 Structural Engineering Analysis and Design Second Edition (iv) The correlation between two random processes can be described using the coherence function. The coherence represents the degree of correlation between two random processes. Two uncorrelated events show zero coherence where as two fully correlated events show unit coherence. The coherence function is defined below as a ratio of the cross-power spectral density function to the geometric mean of the two auto-power spectral density functions. (v) The RMS of the time signal is the square root of the area under the PSD, defining the intensity of the signal. If the mean of the PSD has been removed, the RMS (√m0) is equal to the standard deviation. The mean is almost always removed in dynamic analysis and is dealt with statically. (vi) The peak amplitude of the random signal used to generate the PSD is approximately 3 to 4.5 times the RMS. This is because the amplitude distribution of a narrow or broadband signal is Gaussian. Hence, the peak range is approximately 6 to 9 times the RMS. 414 Structural Engineering Analysis and Design Second Edition 4.6.4.6 MSC.NASTRAN Random Analysis Methodology In random forcing functions, the instantaneous magnitude is not known at any given time. Random vibration excitations include that from earthquake ground motions, wind, ocean waves, acoustic excitations and jet engine noises. A power spectral density (PSD) function defines these random excitations. Frequency response analysis is used to generate transfer functions [H(ω)], which are the ratio of the output to the unit inputs. The input PSDs are then multiplied to the square of these transfer functions [H(ω)] to form response PSDs. The double sided PSD response to a double sided PSD excitation is whilst a single sided PSD response to a single sided PSD excitation is If two processes are correlated then the sequencing effect of the two processes may act to either increase or decrease the overall effects. Thus, the input PSDs must be in the form of auto- and cross-spectral density functions. The double sided and single sided PSD computations are as follows, respectively. The auto- and cross-power spectral density functions may be expressed in matrix form, this permits the rapid calculation of responses using matrix algebra. The auto-power spectral values are located along the leading diagonal while the cross-power terms are located in the remaining cells. Hence the single sided PSD computation is as follows. 415 Structural Engineering Analysis and Design Second Edition To get the transfer function into the correct units for a PSD analysis the response parameter (per unit input loading) has to be squared. This is because the units of PSDs are units of interest squared, per hertz. If one takes the example of an offshore platform the input loading is typically expressed as a sea state spectrum. The process which this PSD defines is the sea surface elevation profile. In the time domain this is the sea surface elevation variation with time. The units of the input PSD are therefore given as m2/Hz (in SI units). Since the response parameter of interest is stress (or strain) the output PSD is usually expressed as MPa2/Hz. The units of the transfer function are therefore given as (MPa/Hz)2. Most of the computational time is spent in solving the structural model. In the time domain, the structural model is solved for each time history of input; hence two load cases would take twice as long to calculate as one. In the frequency domain the linear transfer function is only calculated once, hence two load cases take little more time to analyze than one, and each additional load case can be done virtually instantaneously. The structural calculation is effectively separated from the response analysis when working in the frequency domain. The output from a random response analysis consists of the response PSD, auto-covariance functions, number of zero crossings with positive slope per unit time and RMS values of the response. 416 Structural Engineering Analysis and Design Second Edition 417 Structural Engineering Analysis and Design Second Edition 418 Structural Engineering Analysis and Design Second Edition 4.7 4.7.1 GL, ML Implicit (Real) Modal Transient Response Analysis Nature of the Dynamic Loading Function The solution can be used to ascertain the modal properties of the system by performing a time domain impulse analysis to excite the modes of interest. The duration of the impulse must be sufficiently long to excite the first fundamental mode, which is usually of concern. This would result in a response that includes the first fundamental mode and most likely higher modes as well. The first fundamental mode is readily ascertained from inspection of the response time history curve at any node. Higher natural frequencies can also be ascertained by performing an FFT on the response curve. The solution method can be used to solve dynamic systems subjected to: (a) Deterministic non-periodic short duration impulse (a.k.a. blast) loading functions with subsequent wave propagation (b) Random non-stationary short duration impulse loading functions The force amplitude does not repeat itself regularly but rises from zero to a series of maxima and minima until settling down to a constant value. The starting transient is significant and so the solution is carried out in the time domain. Estimates of the induced stress in a linear elastic body due to an impulsive blast may be made easily in some cases with a simpler static method of analysis. Section 4.7.4 describes this concept further. If the forcing function is a random non-stationary forcing function such that the random forces start from a lowlevel building up to a maximum then dying away, such as in a seismic event, then exact solution methods are not established. Instead, we could either analyze a set of such events using deterministic transient solution methods and then average or envelope the results or alternatively use the crude response spectrum method which envelopes the response spectra of a series of time histories. In this LINEAR TIME DOMAIN solution, the static response must be added to the dynamic response if the dynamic analysis is performed about the initial undeflected (by the static loads) state with only the dynamic loads applied, hence causing the dynamic response to be measured relative to the static equilibrium position. Hence, the total response = the dynamic response + the static response to static loads. Alternatively, in this LINEAR TIME DOMAIN solution, if the dynamic analysis is performed with the deflected static shape as initial input and the static loads maintained throughout the dynamic excitations, the total or absolute response (static and dynamic) is obtained straight away from the dynamic analysis. Hence total response = dynamic response (which already includes the static response to static loads). 4.7.2 Mathematical Formulation of Analysis With the knowledge of the modal frequencies and corresponding mode shapes, the coupled system of simultaneous dynamic equilibrium equations can be uncoupled by premultiplying the dynamic equation of motion by [Φ]T as shown below. This means that the simultaneous ODEs no longer need to be solved simultaneously and so the MDOF system of equations is reduced to a SDOF system of equations, which can be solved independently of each other. The computational benefit comes from not having to run a rigorous simultaneous equation solver. The knowledge of the modal frequencies and the corresponding mode shapes are a prerequisite to this implicit modal transient response analysis, hence the implicit real (note not complex) eigenvalue analysis must be performed first. Because of the fact that the modes are real and do not take into account the explicit elemental (viscous) damping within the structure, the coupled ODEs cannot be uncoupled by [Φ]T. The system of coupled ODEs remains in the existence of viscous damping and the simultaneous equation solver must be invoked. The only difference then between SOL 112 and SOL 109 is the fact that the former solves the equations in the modal coordinates instead of the physical coordinates. Hence, as long as sufficient modes are included (to represent both the static and dynamic response of the system), SOL 112 will give the same solution as SOL 109 even with large values of viscous damping. We know that large values of elemental damping will modify the mode shape and frequencies. However, 419 Structural Engineering Analysis and Design Second Edition a SOL 112 can still be performed because a true (real) modal approach is not undertaken, instead the coupled ODEs are solved using a direct approach, but in the modal coordinates. However, the use of the FREQ4 card, which bases the excitation frequencies to be solved for on the real natural frequencies may prove to be insufficient. This is because with high values of elemental viscous damping, certain local modes can be totally eliminated. For instance, viscous dampers with high coefficients of damping on cables can considerably alter the natural frequency of the local mode and even eliminate a local mode altogether. In this case, the FREQ4 card will not capture the response at the damped natural frequency. Hence, these damped natural frequencies need to be known (by performing a SOL 107) before choosing the excitation frequencies to be solved for using FREQ2 cards. To reiterate, SOL 112 reverts to a direct solution technique (akin to SOL 109) when there is either viscous or structural element damping as the equations of motion cannot be orthogonalized. But the unknowns are still the modal responses and not the physical responses. And because with damping the modes are really complex modes, there is greater difficulty in capturing all the response using the real modes. Hence, even more modes are thus required to capture the response accurately in SOL 112 with element damping especially if the elemental damping is high enough to cause significant complex modes. Thus if elemental damping is high and the modes are complex, the direct method SOL 109 may be more appropriate. If a true modal approach is intended for the solution of coupled ODEs with elemental viscous damping, then a complex modal forced transient response analysis is necessary, although this is quite impractical. The modal matrix from the free, undamped vibration analysis [Φ ] = [{φ}1...{φ}i ...{φ}n ] for the n modes The coupled system of ODEs are given by u&( t )} + [K ]{u ( t )} = {P( t )} [M ]{& Let {u ( t )} = [Φ ]{ξ( t )} [M ][Φ ] & ξ&( t ) + [K ][Φ ]{ξ( t )} = {P( t )} { } Premultiplying by [Φ ]T reduces the coupled system of ODEs to a system of uncoupled ODEs [Φ ]T [M][Φ ] & ξ&( t ) + [Φ ]T [K ][Φ ]{ξ( t )} = [Φ ]T {P( t )} { } Hence the generalised mass matrix and the generalised stiffness matrix for the entire system is the diagonal modal (generalized) mass matrix, [M] = [Φ ] [M ][Φ ] T [ ] the diagonal modal (generalized) stiffness matrix, [K] = [Φ ] [K ][Φ ] = ωn [M] T 2 the modal (generalized) force vector, {P(t)} = [Φ ] {P( t )} The generalized mass matrix and the generalized stiffness matrix are diagonal because of T the orthogonality condition of the normal modes {φi }T [M ]{φ j } = 0 {φi }T [K ]{φ j } = 0 if i≠ j if i≠ j And because these matrices are diagonal, the equations become uncoupled. Accordingly, the generalized mass solitary term and the generalized stiffness solitary term associated with a particular mode ' i' are Mi = {φi }T [M ]{φ i } K i = {φi } [K ]{φ i } = ω2ni Mi T The uncoupled system of equations are thus [M] & ξ&( t ) + [K ]{ξ( t )} = {P(t)} { } These are a set of SDOF ordinary differential equations M& ξ&( t ) + K ξ ( t ) = P (t) for the i th mode i i i i i The central difference numerical integration of the uncoupled equations are then trivial 1 (ξ n +1 − ξ n −1 ) ξ&n = 2 ∆t 1 & ξ&n = 2 (ξ n +1 − 2ξ n + ξ n −1 ) ∆t 420 Structural Engineering Analysis and Design Second Edition and replacing into the dynamic equation of motion averaging the applied force over 3 adjacent time steps 1 (ξ n +1 − 2ξ n + ξ n −1 ) + 1 K i (ξ n +1 + ξ n + ξ n −1 ) = 1 (Pn +1 + Pn + Pn −1 ) 3 3 ∆t 2 Collecting terms and making ξ n +1 the subject Mi A1ξ n +1 = A 2 + A 3ξ n + A 4 ξ n −1 1 1 Mi + K i 3 ∆t 2 1 A 2 = (Pn +1 + Pn + Pn −1 ) 3 2 1 A 3 = 2 Mi − K i 3 ∆t 1 1 A 4 = − 2 Mi − K i 3 ∆t A1 = Once individual modal responses are computed {ξ(t)}, the physical response is thus {u(t)} = [Φ ]{ξ( t )} Since the numerical integration is performed on a small number (as not all the modes are usually included) of uncoupled equations, there is not a large computational penalty for changing ∆t as there is in direct transient response analysis. A constant ∆t is still recommended. In modal transient response analysis, mode truncation refers to not utilizing all the natural modes in computing the response of the structure. At a minimum all the modes that have resonant frequencies that lie within the range of the forcing frequencies have to be retained. For better accuracy, all the modes up to at least 2 to 3 times the highest forcing frequency should be retained. For example, if a structure is excited between 200 and 2000 Hz, all modes from 0 to at least 4000 Hz should be retained as the forcing frequencies still excite the higher modes although not resonating with them i.e. off-resonant excitation. It is thus necessary to evaluate the frequency content of the transient loads and determine the frequency above which no modes are noticeably excited. Truncating highfrequency modes truncates high frequency response. The recommendation of using modes up to 2 or 3 times the highest excitation frequency assumes that the static response can be captured adequately using this finite number of modes. Clearly, if the distribution of applied loads is multiple concentrated forces, then the finite number of modes may still not be sufficient to capture the difficult static shape. In this case, it may be prudent to use static residual vectors instead of increasing the number of vibration modes solely to capture the static response. The following damping models are supported by the solution scheme I. elemental damping i. viscous damping Yes ii. structural damping Specified but converted to viscous II. modal damping i. viscous damping Yes ii. structural damping Specified but converted to viscous III. global proportional viscous damping i. mass proportional damping No ii. stiffness proportional damping Specified but converted to viscous iii. Rayleigh damping No If explicit viscous damping element contributions are made to the damping matrix [C] or if elemental structural damping is specified, then the damping stiffness matrix cannot be diagonalized by the modal matrix. In this case the modal transient response analysis solves the still coupled problem using a direct transient approach but in terms 421 Structural Engineering Analysis and Design Second Edition of the modal coordinates {ξ(t)} instead of the physical coordinates {u(t)}. Since the number of modes used in a solution is typically much less than the number of physical variables, using the coupled solution of the modal equations is less costly than using physical variables. Elemental viscous damping makes contributions to the [C] matrix. T T T [Φ ]T [M ][Φ ]{& ξ&( t )}+ [Φ ] [C][Φ ]{ξ&( t )}+ [Φ ] [K ][Φ ]{ξ( t )} = [Φ ] {P( t )} Elemental structural damping will modify the damping matrix as follows  1 T T T [Φ ]T [M ][Φ ] & ξ&( t ) + [Φ ] [C] + G E [ K E ][Φ ] ξ&( t ) + [Φ ] [K ][Φ ]{ξ( t )} = [Φ ] {P ( t )} ω 4   { } { } ∑ where the parameter ω4 converts the structural damping into equivalent viscous damping as the transient response analysis does not permit the use of complex coefficients. Stiffness proportional global viscous damping modifies the dynamic equilibrium equations as follows T [Φ ]T [M ][Φ ]{& ξ&( t )}+ [Φ ] [C ] +  { }  G T T [ K ][Φ ] ξ&( t ) + [Φ ] [K ][Φ ]{ξ( t )} = [Φ ] {P ( t )} ω3   where the parameter ω3 converts the structural damping into equivalent viscous damping as the transient response analysis does not permit the use of complex coefficients. Hence, with elemental viscous, elemental structural and global structural damping, the uncoupled system of ODEs are given by   1 G ξ&( t ) + [Φ ]T [C] + G E [K E ] + [ K ][Φ ] ξ&( t ) + [Φ ]T [K ][Φ ]{ξ( t )} = [Φ ]T {P( t )} [Φ ]T [M][Φ] & ω4 ω3   The fundamental structural response is solved at discrete times, typically at fixed integration time steps ∆t. Using a central finite difference representation for the velocity and acceleration, { } {ξ& }= 21∆t {ξ n n +1 { } ∑ − ξ n −1 } {&ξ&}= 1 {ξ n +1 − 2ξ n + ξ n −1} ∆t 2 and replacing into the dynamic equation of motion averaging the applied force over 3 adjacent time steps n  1 [Φ]T [M][Φ ]{ξ n +1 − 2ξ n + ξ n −1} + 1 [Φ]T [C] + 1 2 2 ∆t ω4 ∆t  ∑G E [K E ] +  G [K ][Φ ]{ξ n +1 − ξ n −1 } ω3  1 T [Φ] [K ][Φ]{ξ n +1 + ξ n + ξ n −1} = 1 [Φ]T {Pn +1 + Pn + Pn −1} 3 3 Collecting terms and making {ξ n +1 } the subject + [A1 ]{ξ n +1} = [A 2 ] + [A 3 ]{ξ n }+ [A 4 ]{ξ n −1}  1  [M ] + 1 [C] + 1 2 2 ∆t  ω4  ∆t [A1 ] = [Φ ]T  ∑G E [K E ] +  1  G [K ] + [K ][Φ ] ω3  3  [A 2 ] = 1 [Φ]T {Pn +1 + Pn + Pn −1} 3 [A 3 ] = [Φ ]T  2 [M ] − 1 [K ][Φ ] 2 3   ∆t   1 [M] + 1 [C] + 1 2 2∆t  ω4  ∆t [A 4 ] = [Φ]T − ∑G E [K E ] + 422  1  G [K ] − [K ][Φ ] ω3  3  Structural Engineering Analysis and Design Second Edition The modal transient response analysis solves the still coupled problem using a direct transient approach but in terms of the modal coordinates {ξ(t)} (modal responses in modal space) instead of the physical coordinates {u(t)}. A constant ∆t is obviously computationally beneficial. Hence, if discrete damping is desired, direct transient response analysis is recommended. If however only viscous modal damping ζi is specified, the generalized damping matrix [Φ]T[C][Φ] remains diagonal and so the uncoupled equations of motion can be maintained. The uncoupled equations of motion become for the i th mode M& ξ&( t ) + (ζ 2M ω )ξ& ( t ) + K ξ ( t ) = P (t) i i i i ni i i i i which is solved for the individual modal responses ξi(t) using the Duhamel’s Integral   ξ& ( τ = 0) + ξ i ( τ = 0)ζ i ω ni ξ i ( τ = t ) = e −ζ i ωni t  ξ i ( τ = 0) cos ω di t + i sin ω di t  ω di   τ = t 1 + Pi ( τ)e −ζ i ωni ( t − τ ) sin ω di (t − τ )dτ τ = 0 M i ω di ∫ where ω di = ω ni 1 − ζ i2 If structural modal damping Gi is specified, it is converted to an equivalent viscous modal damping ζi = G i / 2 423 Structural Engineering Analysis and Design Second Edition 4.7.3 Capability of A Finite Number of Modes To Model The Static and Dynamic Response of Structure First and foremost, the chosen modes must cover and extend beyond the excitation frequency range such that both the resonant response of the modes within the range and the off-resonant response of the modes beyond (from say a 1/3rd of lowest excitation frequency to 3x the highest excitation frequency determined by FFT as frequency content not obvious) the range are captured. This will sufficiently model the dynamic response. Considerations then must be made for the finite number of modes to capture the static response. Modal truncation can be specified by delimiting the number of modes used in the response calculations from that calculated by EIGRL. To delimit the natural modes employed, LFREQ (lower limit of the frequency range), HFREQ (upper limit of the frequency range) or LMODES (number of lowest modes retained) can be used. To determine if enough modes have been selected to represent the static response of the structure, a dynamic load curve ramped up gradually from zero to a constant value can be applied to a SOL 112 and the final static equilibrium response after all the dynamic amplification effects have subsided can be compared to the static response from a SOL 101 solution. Often, if the finite number of modes is found to be capable of representing the static response, then they will usually be found to be sufficient to represent the dynamic response as well. To determine if enough modes have been chosen to represent the static and dynamic response of the structure, a SOL 112 solution can be compared to that of a SOL 109 and the response time history traces compared. The relative contribution of each mode to the total static and dynamic response can also be determined. This is known as the modal responses, i.e. the value of the modal variables in the modal solution scheme. The Case Control Cards SDISP, SVELO and SACCE will produce the modal solution set output, {ξi(t)}. These are plots of the modal response (for each mode) in terms of time, i.e. the time domain modal response. That is to say, SDISP(PUNCH) (or SVELO or SACCE) will output one value for each mode at each time step. These are the modal responses in modal space. They must be multiplied by the corresponding mode shapes in order to obtain the modal responses in physical space i.e. {ui(t)} = {φi}ξi(t) Another method of determining the modal contribution of individual modes to a particular excitation is by using the modal strain energy. Firstly, to evaluate the ability of the natural modes to represent the static response, a SOL 101 is run with the amplitude of the dynamic loads applied as a static load and the results are written to a DMIG file using the alter pchdispa.v2001. Then a SOL 103 us run with the DMIG included and also the alter modevala.v2001 to ascertain how well each and every mode can represent the static solution. The strain energy for each mode can be compared to the strain energy in all the modes calculated and also the input vector. Note that the eigenvector scaling must be set to the default MASS (not MAX) for this alter to be valid. Secondly, to evaluate the ability of the natural modes to represent the dynamic response, the alter mtranea.v2001 is utilized for SOL 112. Note that the capability of a finite number of modes to represent the static and dynamic response of the structure is limited to a particular force excitation direction and distribution. If the force changes its location or direction, then the prominence of the different modes which will be different. This is simply because changing the location or direction of the force will cause a different set of modal forces and hence a different level of excitation of the different modes. The capability of a finite number of modes to represent the static and dynamic response of the structure depends also on the level of elemental structural (although cannot be accounted for exactly in the time domain) and elemental viscous damping present within the system. This is because, the level of elemental damping affects the complexity of the modes, hence possibly requiring more real modes if the modal complexity is high. Thus damping should be included when performing the study to determine the required number of modes. The above method assumes that the direct solution SOL 109 is exact and hence we only have to match that using a certain number of modes. However, there is an instance when the solution from the direct approach SOL 109 is inaccurate. This occurs when there is elemental structural damping. This problem does not occur in the 424 Structural Engineering Analysis and Design Second Edition frequency domain and the approach of comparing the modal estimate to the correct direct solution can be always made. It can also always be made in the time domain if the only form of damping is viscous. However, time domain solutions cannot model structural damping exactly, hence having to convert the structural damping into equivalent viscous damping. But this conversion ties the equivalence to one natural frequency (PARAM, W3 or PARAM, W4). Hence the damping will only be accurate for the mode with the natural frequency corresponding to (PARAM, W3 or PARAM, W4), that to only at that excitation frequency, but then again damping is most critical at resonance. But the fact of the matter is that the direct solution will not be accurate when there is structural damping. Hence, noting that the direct solution is not a good benchmark to measure against, a modal approach must be used. Employing SOL 112, a solution would be to insert modal damping estimates based on a SOL 107 calculation. Hence different modes will be damped accurately (but again not at all excitation frequencies, this usually being an acceptable inaccuracy). The following graph shows the modal structural damping for a bridge with a floating track slab resting on isolation pads. The graph below shows significant high frequency response when modal damping (with no elemental structural damping) is applied in a SOL 112 solution compared to a highly attenuated high frequency response in a SOL 109 direct solution which incorporates equivalent viscous damping for elemental structural damping tied in at the frequency of the first mode. Thus clearly, a modal approach must be used when structural damping is present. Alternatively of course, a direct time domain analysis can be performed if Rayleigh damping (which damps two modes accurately and interpolates for the modal damping within the range) is incorporated. 425 Structural Engineering Analysis and Design Second Edition But let us go with the modal solution. Now since no comparison to a direct approach can be made, the verification the sufficiency of the chosen number of modes becomes difficult. A solution may be to run repetitive modal SOL 112 analysis (of course with the modal damping from SOL 107 incorporated, but no elemental structural damping achieved by simply excluding PARAM, W3 and/or PARAM, W4) with increasing number of modes until convergence of the results occurs. But the question then becomes, does the results converge to the true solution? It would then be prudent to compare the modal results with gradually increasing number of modes with the SOL 109 solution with ‘tied in’ equivalent viscous damping, bearing in mind that we would expect to see high frequency response in the modal solution. The following graphs show such a comparison. A significant observation can be made by looking at these graphs. Although the chosen modes cover and extend beyond the excitation frequency range such that both the resonant response of the modes within the range and the off-resonant response of the modes beyond the range are captured, clearly something is amiss for there to be such a difference in the response. Now if the chosen modes cover the excitation frequency range adequately, the only reason for there to be any inaccuracy in the modal solution is if the modes still (for whatever reason) are not sufficient to capture the static response. This can occur if the distribution of the force is such that the static response (i.e. the static deflected shape of the structure to the applied loads) is too complicated for it to be represented by the dynamic eigenvectors. In the above example, the dynamic eigenvectors were not sufficiently enough to capture the static response of a passing train on a bridge. Because of the nature of the load distribution being concentrated loads applied at certain closely spaced intervals, the static response is clearly a wave-like shape of a low wavelength. Imagine the static response of the bridge to the train passing to be the train stationary at intervals along the bridge. The graph above did not have sufficient modes to capture this somewhat difficult shape that can possibly be captured by higher frequency modes. This proves to be correct and the comparison is shown below where the SOL 112 solution with modes up to 200Hz seem to converge to the correct solution. 426 Structural Engineering Analysis and Design Second Edition Clearly then, instead of laboriously calculating modes of such high frequency to capture the static response, surely it is better to use static residual vectors instead that capture the static response straight away. Indeed! So long as the dynamic modes are chosen to cover and extend beyond the excitation frequency range (say 2x or 3x the highest excitation frequency determined by FFT for time domain loading functions as frequency content not always obvious) such that both the resonant response of the modes within the range and the off-resonant response of the modes beyond the range are captured, it is highly recommended to append the static residual vectors to the total response. Static residual vectors (PARAM, RESVEC, YES) can be calculated except when using the seismic large mass method for enforced motion. The residual vector method is more efficient than the mode acceleration method and can be applied to both superelements and the residual structure when substructuring is employed. Clearly though, there should be sufficient modes comfortably beyond within the excitation frequency bandwidth to capture the dynamic response, and the static residual vectors should only be used as a final step to append the quasi-static responses of high frequency (relative to the excitation frequencies) modes. There is no question of damping associated with these static vectors, as by definition they are the static response of high frequency modes i.e. the response of high frequency modes to low (relatively that is) frequency excitation. The response then is quasi-static and by definition independent of the damping of the mode. The effect (i.e. the no amplification response or rather the quasi-static response) of these truncated high frequency modes can thus be approximated by residual vectors. These vectors are by default created using the applied loads and solving for the static response in a static solution. The following graph shows the effect of using these static residual vectors in the above train passing problem. Clearly, the true solution was obtained using modes up to just 50Hz with PARAM, RESVEC, YES included. Even the SOL 112 solution with 100Hz (without RESVEC) was still not able to capture the true response, but is moving in the right direction since as shown modes up to 200Hz may just be sufficient to capture the static response. Hence RESVEC is highly recommended. Only when the static response is adequately captured will derived quantities from the response be accurate. For instance, modal damping estimates from signal filtering the response (to only include the mode of interest and doing a logarithmic decrement calculation) will only be accurate when the static response is adequately captured. There are of course much better methods of computing the modal damping. Note that SOL 112 reverts to a direct solution technique (akin to SOL 109) when there is either viscous or structural element damping as the equations of motion cannot be orthogonalized. But the unknowns are still the modal responses and not the physical responses. And because with damping the modes are really complex modes, there is greater difficulty in capturing all the response using the real modes. Hence, even more modes are thus required to capture the response accurately in SOL 112 with element damping especially if the elemental damping is high enough to cause significant complex modes. Thus if elemental damping is high and the modes are complex, 427 Structural Engineering Analysis and Design Second Edition the direct method SOL 109 may be more appropriate although of course modal damping cannot be utilized and hence there is a genuine difficulty in modelling structural damping accurately. The convergence of average stress values is quite similar to the convergence of velocities4. However, for structures with any form of stress concentrations, it is not the average stress that is of concern, but the peak stresses. These involve small local regions of high strain energy with low relative velocities around the stress concentration. It follows from the consideration of the Rayleigh quotient that such behavior will be associated with high frequency modes and the low frequency ones will not excite the stress concentrations very strongly. Hence, if any form of condensation (reduced number of modes, Guyan reduction, dynamic substructuring or large time steps that filter high frequency modes in implicit time integration schemes) is used to calculate the dynamic response, then this will filter out the peak stresses. This condition arises when the stresses are determined directly from the displacement response. The peak stresses will be under-estimated even if mesh refinement was undertaken, since the error is directly related to the degree of condensation of the high frequency modes and not upon the mesh density. The user can test the accuracy of the dynamic stress recovery process by simulating the static response in the dynamic solution (zero frequency excitation for the frequency domain or dynamic relaxation for time domain). This can then be compared to the stress distribution produced directly from a true static analysis. If the comparison is good, then the dynamic stress recovery procedure is verified. We shall discuss the methods of improving the modal solution accuracy. We shall discuss the I. matrix method or the mode displacement method II. mode acceleration method III. mode truncation augmentation method i.e. the static residual RESVEC method (MT) The dynamic equilibrium equation is presented. [M ]{& u&( t )} + [C]{u&( t )} + [K ]{u ( t )} = {P( t )} = {P0 }P( t ) The applied loading is composed of two parts, {P0} is the invariant spatial portion and P(t) is the time varying portion. The matrix method (default) (PARAM, DDRMM, 1) computes displacements and stresses per mode and then computes physical displacements and stresses as the summation. Cost is proportional to number of modes. Since the number of modes is usually much less than the number of excitation frequencies (or time steps in the time domain), the matrix method is usually more efficient. The mode displacement method (PARAM, DDRMM, −1) computes the total physical displacements for each excitation frequency (or time step in time domain) from the modal displacements, and then computes the element stresses from the total physical displacements. Cost is proportional to the number of excitation frequencies (or time steps in time domain). The coupled system of ODEs are given by [M]{& u&( t )} + [C]{u&( t )} + [K ]{u ( t )} = {P( t )} Let {u ( t )} = [Φ ]{ξ( t )} [M][Φ ] & ξ&( t ) + [C][Φ ] ξ&( t ) + [K ][Φ ]{ξ( t )} = {P( t )} { } { } Premultiplying by [Φ ] T T T [Φ ]T [M ][Φ ] & ξ&( t ) + [Φ ] [C][Φ ] ξ&( t ) + [Φ ] [K ][Φ ]{ξ( t )} = [Φ ] {P( t )} These equations are solved for {ξ( t )} as a set of SDOF systems if the damping matrix can be orthogonalized, T { } { } otherwise directly using a simultaneous equation solver. Finally the physical response is recovered as follows. {u(t)} = [Φ ]{ξ( t )} {u&(t)} = [Φ ]{ξ&( t )} {& u&(t)} = [Φ ]{& ξ&( t )} 4 NAFEMS. A Finite Element Primer. NAFEMS Ltd., Great Britain, 1992. 428 Structural Engineering Analysis and Design Second Edition A key concept of the matrix method or the mode displacement method is that the displacement, velocity and acceleration modal responses were obtained from equations which were decoupled (or attempted to be decoupled) by pre-multiplication by {Φ}T. The load vector was also pre-multiplied by {Φ}T. This clearly thus limits the representation of the applied loading to be dependent on the chosen number of dynamic modes. The choice of the number of modes retained is typically driven by the need to span the frequency content of interest. That is, the frequency of the highest mode retained should sufficiently exceed the frequency content of the applied time history by a predetermined margin (say 2x or 3x highest excitation frequency). However, this criterion only addresses the time dependent portion of the applied loading, P(t) and ignores the spatial portion {P0}. These result in accuracies especially if the spatial distribution of the loading is concentrated and repetitive such that the lower dynamic modes have difficulty in capturing the response. The truncated spatial portion of the applied loading due to the finite number of dynamic modes can be quantified as follows. The exact spatial loading is {P0}. To obtain the modal representation of the spatial loading, the static equation must be considered. The static equation [K ]{u} = {P0 } Let {u} = [Φ ]{ξ} [K ][Φ ]{ξ} = {P0 } To obtain {ξ}, premultiplying by [Φ ]T [Φ ]T [K ][Φ ]{ξ} = [Φ ]T {P0 } [Φ ]T {P } [Φ ]T {P0 } {ξ} = T 0 = [Φ ] [K ][Φ ] {ω 2 } Hence, on substituti on T [ Φ ] {P0 } [K ][Φ ] 2 = {P0 } {ω } { } But from eigenvalue problem [K ][Φ ] = [M ][Φ ] ω 2 , hence the modal representation of spatial load [M ][Φ ]{ω 2 }[Φ ] {2P0 } = {P0 } T {ω } [M ][Φ ][Φ ]T {P0 } = {P0 } We conclude that the truncated part of the spatial portion of the applied load is {PT } = {P0 } − [M ][Φ ][Φ ]T {P0 } Clearly, as the number of modes is increased, the truncated part {PT} becomes smaller. However, the number of modes required for an accurate solution can become significant, possibly negating the computational advantages gained by the modal truncation method. Mode acceleration method (PARAM, DDRMM, −1 and PARAM, MODACC, 0) is a method of improving the modal solution in the time or frequency domain. A much better estimate of the peak stress can be obtained using the mode acceleration method. Here the acceleration and velocity response is first obtained. The modal solutions are expanded to analysis set vectors and multiplied by the mass, damping and direct input matrices to generate equivalent loading vectors. These vectors are added to the applied load function to generate a pseudo load matrix for all selected frequencies (or time steps in the time domain). The static problem is then solved using a static analysis procedure. The stresses are found from solving this static problem. The mode acceleration method considers higher modes and hence gives more accurate answers than the matrix method or the mode displacement method especially if the number of retained modes is small in comparison to the number of DOFs. The accuracy of the dynamic stress distribution will then be comparable to that of a static analysis. The method works because the high frequency modes that define the stress concentration have a constant response over the low frequency excitation range that has been considered for the dynamic calculation, and since the stresses are found from an 429 Structural Engineering Analysis and Design Second Edition instantaneous static sum, the constant component of the high frequency response have been included. In other words, the higher modes respond in a quasi-static manner to lower frequency excitations. Hence, at lower frequency excitations, the inertia and damping forces contain little contribution from higher modes. Also, the relative accelerations around the stress concentration are low and all that is required is a reasonably accurate estimate of the overall structural accelerations. This will be given by the lower modes 5. The overall performance and accuracy of the mode acceleration method falls somewhere between the standard modal output and the expensive direct solution method. It is then of course not cost-effective when only the peak displacements are important. The logic of the mode acceleration method is clear, if the number of modes retained accurately spans the frequency range of interest, any loading represented by the non-retained modes will produce a quasi-static response. Consequently, the response due to the non-retained modes will have no dynamic amplification. That is to say, the modes not retained will cause no appreciable velocity or acceleration response and hence the velocity and acceleration response can be obtained using the matrix or mode displacement method whilst the displacement response is obtained using a more direct approach. From [Φ ]T [M ][Φ ]{& ξ&( t )}+ [Φ ]T [C][Φ ]{ξ&( t )}+ [Φ ]T [K ][Φ ]{ξ( t )} = [Φ ]T {P( t )} In modal acceleration method, damping need not be specified for the higher unretained modes as the displacement response is {& u&(t)} = [Φ ]{& ξ&( t )} independent of damping of the However, the displacement response is obtained directly from higher unretained modes, but of −1 −1 −1 & & & course dependent on damping of {u(t)} = [K ] {P( t )} − [K ] [M ][Φ ] ξ(t ) − [K ] [C][Φ] ξ(t ) retained modes. A key concept of the mode acceleration method is that although the velocity and acceleration modal responses were obtained from equations which were decoupled (or attempted to be decoupled) by premultiplication by {Φ}T with the load vector also pre-multiplied by {Φ}T, the displacement response was obtained directly from the equilibrium equation without pre-multiplication by {Φ}T. This is done because it is assumed that there is no appreciable velocity or acceleration response due to the applied loading from the unretained modes, but there will be an appreciable quasi-static displacement response due to the applied loading from the unretained modes. Hence not only are modal coordinates used to determine the modal velocity and acceleration responses, but the contribution of velocity and acceleration in the direct displacement response expression is also in modal terms as shown above. The modal velocity and acceleration response is determined as before {u&(t)} = [Φ ]{ξ&( t )} { } { } Mode truncation augmentation method i.e. the static residual RESVEC method (PARAM, RESVEC, YES or PARAM, RESVINER, YES) is an excellent method of improving the modal solution in the time or frequency domain. It attempts to correct for the inadequate representation of the spatial loads in the modal domain by creating additional “pseudo eigen” or static residual vectors to include in the modal set for the response analysis. The terminology of “pseudo eigen” is used because the static residual vectors are orthogonal to on the mass and stiffness matrices but do not satisfy the eigenvalue problem. The mode truncation vectors are created using a mathematically consistent Rayleigh-Ritz approximation where the assumed Ritz basis vectors are derived using the spatial force truncation vector {PT} presented above. The mode truncation vectors are orthogonal to the retained eigenvectors since the force truncation vector does not contain any components of the retained eigenvectors. For the response solution the mode truncation vectors and associated Rayleigh-Ritz frequencies are appended to the retained eigenvectors and the modal response analysis proceeds as f the augmented vector set were all eigenvectors. A mode truncation vector is first determined by solving for the displacement vector {X} [K]{X} = {PT} 5 NAFEMS. A Finite Element Primer. NAFEMS Ltd., Great Britain, 1992. 430 Structural Engineering Analysis and Design Second Edition Form, [K ] = [X] [K ][X] [M ] = [X] [M][X] T T and solve the reduced eigenvalue problem [K ]{Φ } = [M ]{Φ }ω R R 2 S Finally, the static residual vectors can be determined from {Φ S } = {X}{Φ R }T These static residual vectors are simply appended to the retained modal set for the response calculations. There will be one static residual vector for each spatial load vector, i.e. one for each time step. Finally, the static residual vectors can be determined from {Φ AUGMENTED } = Φ RETAINED DYNAMICMODES + {Φ S } { } The coupled system of ODEs are given by [M]{& u&( t )} + [C]{u&( t )} + [K ]{u ( t )} = {P( t )} Let {u ( t )} = [Φ ]{ξ( t )} [M][Φ ] & ξ&( t ) + [C][Φ ] ξ&( t ) + [K ][Φ ]{ξ( t )} = {P( t )} { } { } Premultiplying by [Φ ] T T T [Φ ]T [M ][Φ ] & ξ&( t ) + [Φ ] [C][Φ ] ξ&( t ) + [Φ ] [K ][Φ ]{ξ( t )} = [Φ ] {P( t )} These equations are solved for {ξ( t )} as a set of SDOF systems if the damping matrix can be orthogonalized, T { } { } otherwise directly using a simultaneous equation solver. Finally the physical response is recovered as follows. {u(t)} = [Φ ]{ξ( t )} {u&(t)} = [Φ ]{ξ&( t )} {& u&(t)} = [Φ ]{& ξ&( t )} PARAM, RESVEC, YES augments static residual vectors due to the applied loads (one residual vector for each time step). PARAM, RESVINER, YES augments static residual vectors due to inertial loads i.e. unit accelerations of mass (6 residual vectors created for inertial loads in the 6 DOFs). RESVINER is not as good as RESVEC unless the loading is gravitational loads. The Rayleigh-Ritz frequencies are printed in the .f06 file. These frequencies will be higher than those of the real dynamic modes. Modal augmentation vectors by PARAM, RESVEC, YES are must be used for modal methods (in the time or frequency domain) with enforced motion. This is because since there no rigid body modes (as they are constrained by the enforced motion), there can be no motion of the enforced points unless RESVEC is used. A key concept of the mode truncation method is that the truncated force captured by the static residual vectors include dynamic effects from the non-retained modes, including velocity and acceleration effects. This is unlike the mode acceleration method which does not consider the velocity and acceleration response of the unretained modes, only the displacement response. The mode truncation method attempts to average in a consistent mathematical sense the response of all the modes not retained into a single static residual vector (for each load case or time step) which contributes to the static displacement and the dynamic velocity and acceleration response. The mode acceleration method forces the higher unretained modes to respond only statically. Hence the mode acceleration method is a subset of the mode truncation method. Also, since dynamic response is accounted for, unlike the mode acceleration method, damping must be specified for the higher unretained modes in the mode truncation method. This effect should however be small as sufficient dynamic modes (say 2x or 3x highest excitation frequency) should be requested to capture the amplified response where damping really matters. 431 Structural Engineering Analysis and Design Second Edition A highly illustrative concept is the modal response concept. This can be punched using SDISP, SVELO or SACCE. These are really the plots of the solution set. Below is a plot of the dynamic modal responses without the static residual vectors multipliers. Note that the eigenvectors were normalized using MAX, thus the plot shows the significant modes. These plots will be meaningless if MASS normalization was used. The following graph then shows the solution set responses including both the dynamic modal responses and the static residual vectors multipliers (although the comparison should only be made if the method of eigenvector normalization is consistent). Clearly the static residual vectors are quite significant in this particular case. Another method of determining the adequacy of the finite number of modes is to evaluate the cumulative effective mass (NASTRAN Case Control Command MEFFMASS) of the chosen number of modes. The effective mass has got a specific meaning in seismic analysis, but can be used for other dynamic analyses as well as a measure of determining the adequacies of the finite number of modes. A cumulative effective mass that approaches unity suggests adequacy of the chosen modes to model the spatial distribution of the loading. This parameter of course does not say much about the adequacy of the chosen modes to model the frequency content of the loading. Essentially, and to reiterate, the chosen number of modes must be sufficient to model both the frequency content and also the spatial distribution of the loading. It is found that for a high cumulative effective mass, uniformly distributed loads such as in seismic analyses require only a few modes whereas a concentrated patch requires more modes and finally a highly concentrated load requires a much greater number of modes to capture the effect of the spatial distribution of the loading. 432 Structural Engineering Analysis and Design Second Edition 4.7.4 Concepts of Equivalent Static Force In large structural engineering projects, it may be more convenient to derive appropriate equivalent static forces for the dynamic effects of certain types of excitations. Codes of practice usually derive equivalent static loads from dynamic considerations for application in linear static analyses of large structural engineering finite element models. This may be used for instance in the impact analysis of a train in the design of an underground station. The impacting train imposes an impulse I = F∆t = m∆v onto the structure, where m and ∆v are known. Knowing that F∆t is the area under the impulse curve, making an estimate of the shape of the impulse curve and the duration ∆t, we can thus estimate the peak amplitude, p0. Hence, the impulse curve is defined. Now, we know that the true dynamic response is given for mode i as p p ξ i ( t ) = D i ( t ) 0i = D i ( t ) 2 0i Ki ω ni M i {u i ( t )} = {φ i }ξ i ( t ) To derive an equivalent static response to a dynamic excitation we need to make the assumption that the DYNAMIC AMPLIFICATION and the SHAPE of the response are governed primarily by the FUNDAMENTAL MODE. Let us illustrate this concept. A set of static equilibrium equations can be transformed from physical coordinates into modal coordinates by the same methods transforming dynamic equilibrium equations into modal coordinates. This is described in Section 3.1.4. If ALL the modes are included, then there will be the same number of modal DOFs to the physical DOFs and the computational problem size is exactly the same. The response will also be exactly the same between the physical model and the modal model. This concept is also demonstrated when we observe the 0.0 Hz (or close to) point on the frequency response function (FRF) of a SOL 108 and SOL 111 analyses. The SOL 108 uses all the modes (because it solves the frequency domain dynamic equilibrium equations in the physical coordinates) whilst SOL 111 employs only the user-selected modes. Hence, a SOL 108 FRF a 0.0 Hz (assuming no structural damping) would give the same response as a static analysis SOL 101, whilst a SOL 111 would not. As more modes are employed the SOL 111 result will approach that of the true static response. These concepts are presented in Section 4.3.3. Now we know that the static response will include all the modes. So, what about the dynamic amplification? Because the method of solution of a set of static equilibrium equations is direct (and not modal), different modes cannot be amplified uniquely. We are thus resolved to amplifying all the modes by the same dynamic amplification factor, Di(t). We choose the FUNDAMENTAL MODE because it is features most prominently in the static response by virtue of having the largest p0i/Ki term as higher modes will have larger modal stiffness Ki terms. This is another way of simply saying that is because the static deformed shape usually somewhat resembles that of the fundamental mode because the static response of higher modes are much smaller. Hence the dynamic amplification D1(t) is based upon the ratio of the duration of the impulse, ∆t with respect to the period of the fundamental period, T1. And thus we can estimate the maximum dynamic amplification D1max. The equivalent modal static force will thus be D1maxp0i and a linear static analysis is subsequently carried out with loading of D1maxp0 (where p0 is the amplitude of the applied dynamic force) to approximate the dynamic response. Response Spectrum 2.5 2 Dimax 1.5 1 0.5 0 0 0.5 1 1.5 2 2.5 3 td/Ti 433 3.5 4 4.5 Structural Engineering Analysis and Design Second Edition Reiterating, performing an equivalent static analysis to approximate the dynamic response makes the assumption that the DYNAMIC AMPLIFICATION of ALL the modes is based upon that of ONLY the FUNDAMENTAL MODE and hence ignoring the POTENTIALLY LARGE AMPLIFICATIONS OF HIGHER MODES. Even if the highest amplification factor MAX[Dimax] considering all modes i (note that the amplification factor is theoretically limited to 2.0) were to be employed, it is not necessary that the static solution will always be safe. This is because, due to the fact that all the modes have to be amplified by the same amplification, the SHAPE of the response will be governed by the fundamental mode (due to its lowest Ki term). The familiar higher mode rippled shape (which may certainly cause greater stressing in some elements) will not be observed as that would require a greater amplification of a particular higher mode and not (the fundamental mode and) all higher modes, the consequence of which is a canceling of response that cause the ripple effect. Take for instance the green triangular impulse loading function of duration td. If td/T1 ≈ 1.0, then the greatest dynamic amplification Di is observed on the fundamental mode and higher modes observe lower amplifications. The AMPLITUDE and SHAPE of the response will be governed by the fundamental mode and hence the equivalent static procedure may be justified. However, if td/T1 is << 1.0, then the greatest amplification Di is observed by some higher mode i which has td/Ti ≈ 1.0 and not by the fundamental mode. Note that if td/T1 is < 0.2, then the maximum modal response due to the first mode can be approximated as follows. ξ1 (τ = t ) = h(t - τ) ξ1 max = 1 M1ω n1 ∫ ξ1 max = 1 M1ω d1 ∫ τ= t τ =0 τ= t τ =0 ∫ τ= t τ= 0 p( τ)dτ φ i p( τ)dτ undamped φ i p( τ)dτ damped where φ i = mod al component at excitation point The maximum modal displacement response is I/(ωd1M1). The magnitude of the impulse I can be calculated as m∆v where m is the small mass and ∆v the change of velocity at impact. If there is no rebound ∆v is the approach velocity. The maximum modal velocity response is approximately I/M1 and acceleration is approximately Iωd1/M1. Anyway, using the amplification of the fundamental mode to represent the amplification of all modes (in the equivalent static procedure) will not be conservative. Even if the amplification for this particular higher mode was used to represent the amplification for all the modes (including the fundamental mode), there is no guarantee that the stressing of all the elements within the system will be on the conservative side. This is because, as mentioned, the exclusive amplification of that particular (rippling) mode shape (or eigenvector) which observed the greatest amplification cannot be made in an equivalent static procedure. Instead the amplification of all the modes with this single amplification factor causes the ripple effect (which may have caused certain elements to witness greater stresses) to be ineffectual as a canceling of response occurs. Hence, if td/T1 is << 1.0, the equivalent static procedure may NOT be safe. 434 Structural Engineering Analysis and Design Second Edition 4.7.5 Structural Damping in Time Domain Analyses Direct frequency domain solution SOL 108 can handle both elemental structural and elemental viscous damping exactly. All modes are correctly damped at all excitation frequencies. Modal frequency domain solution SOL 111 reverts to a direct approach (but in the modal coordinates) when there is either elemental structural or elemental viscous damping. Clearly, the solution is not exact because of modal truncation. If the number of modes were increased to equal the number of DOFs, then the solution will be exact as obtained by SOL 108. But if a finite number of modes less than the number of DOFs are used, then the solution will be approximate. If the modes are only slightly complex, then the real modes (which are used in SOL 111) can easily capture the true complex modes. But if the modes are very complex (quantified on the complexity plot), then even more (real) modes are necessary to capture the true complex modes. In either case, SOL 111 can be used (as it reverts to a direct approach) so long as the number of modes is sufficient to capture the static and dynamic response accurately. A further method can be employed if the modes are only mildly complex, i.e. the response calculations can be performed using SOL 111 with modal damping estimates obtained from SOL 107. SOL 107 can be used to calculate the modal damping from a model with elemental structural and/or viscous damping. These modal damping (in structural or viscous form) estimates can be employed within a SOL 111 analysis, but of course removing the elemental structural and/or viscous damping so not as to double count. SOL 111 in this case will not revert to SOL 108 as there is only modal damping. Note that the modal damping can be processed as either structural or viscous damping (according to PARAM, KDAMP). This conversion of modal damping from structural to viscous and vice versa is actually only perfectly accurate when the frequency of excitation matches the natural frequency of the mode (at resonance), but of course this is acceptable as only that is the instance when the damping estimate is most critical. Hence this method will damp the different modes accurately, but not at all excitation frequencies. The benefit of this approach is only computation speed as the solution can be performed in modal space using a modal approach. If the modes are found to be complex, then the user can always revert to the direct SOL 108 which can handle both structural and viscous damper elements accurately anyway. Time domain solution cannot handle structural damping exactly, only viscous damping. A direct transient analysis SOL 109 or a modal transient analysis SOL 112 correctly models elemental viscous damping at all modes and at all excitation frequencies. SOL 109 and SOL 112 however do not model elemental structural damping (specified on the GE field of the MAT1 card or can be specified also using CELAS or CBUSH) exactly. If structural damping is specified at the element levels, then the incorrect modal damping will result because the conversion from structural to viscous damping will only be valid for one modal natural frequency, w4 as specified by PARAM, W4. A solution may be to use a modal approach. Now, the modal transient response analysis SOL 112 reverts to a direct approach (but in the modal coordinates) when there is either elemental structural or elemental viscous damping. Clearly, the solution is not exact because of modal truncation added to the fact that elemental structural damping cannot be incorporated exactly in a time domain solution. If the number of modes were increased to equal the number of DOFs, then the solution will be exactly as obtained by SOL 108, but still not exact theoretically due to the incorrect modelling of elemental structural damping. Certainly, if a finite number of modes less than the number of DOFs are used, then the solution will be even more approximate. If the modes are only slightly complex, then the real modes (which are used in SOL 112) can easily capture the true complex modes. But if the modes are very complex (quantified on the complexity plot), then even more (real) modes are necessary to capture the true complex modes. In either case, SOL 112 can be used (as it reverts to a direct approach) so long as the number of modes is sufficient to capture the static and dynamic response accurately, but this still does not correctly model structural damping in the time domain solution. Modelling elemental structural damping mechanism in the time domain using an equivalent viscous damping will certainly over-damp higher modes of vibration. A method can be employed if the modes are only slightly complex i.e. the response calculations can be performed using SOL 112 with modal damping estimates obtained from SOL 107. SOL 107 can be used to calculate the modal damping from a model with elemental structural and/or viscous damping. These modal damping (of course internally converted to the mathematical viscous form irrespective of whether specified as modal viscous damping or modal structural damping) estimates can be employed within a SOL 112 analysis, but of course removing the elemental structural and/or viscous damping so not as to double count. SOL 112 in this case will not revert to SOL 109 as there is only 435 Structural Engineering Analysis and Design Second Edition modal damping. Note that the modal damping must be processed as viscous damping in this time domain solution. This conversion of modal damping from structural to viscous and vice versa is actually only perfectly accurate when the frequency of excitation matches the natural frequency of the mode (at resonance), but of course this is acceptable as only that is the instance when the damping estimate is most critical. Hence, this modal method SOL 112 offers the advantage of more correctly modelling the elemental structural damping on the different modes, although the modes are not damped accurately at all excitation frequencies. Since modal damping is explicitly calculated and applied, all the modes are correctly damped by the elemental structural damping here in the time domain. Note that this method of employing modal damping is valid only if the modes are only slightly complex as the modal damping values are applied onto the real modes. If the modes are highly complex, then elemental structural damping cannot be incorporated exactly in the time domain. The graph shows two traces, the first obtained from a SOL 109 solution with equivalent elemental viscous damping for elemental structural damping tied in at the first mode, and the second showing the solution obtained using a SOL 112 with no elemental damping (hence equations can be orthogonalized) but with modal damping. Clearly, there is significant response from the higher frequency modes, a feature that will be masked if equivalent viscous damping and the direct solution were used. 436 Structural Engineering Analysis and Design Second Edition 4.7.6 MSC.NASTRAN Decks 4.7.6.1 GL, ML Modal Forced Transient Response Analysis $ EXECUTIVE CONTROL SECTION SOL 112 $ CASE CONTROL SECTION $ Sets defining grid ids or element ids SET < Number > = 1 THRU 100, 211, 343, < etc > $ Grid output of displacement, velocity and acceleration with time $ SORT1 lists the results by time whilst SORT2 lists the results by grid id DISPLACEMENT(,) = ALL/ VELOCITY(,) = ALL/ ACCELERATION(,) = ALL/ $ Grid output of applied load vector OLOAD(,) = ALL/ $ Grid output of modal responses (in modal space) SDISPLACEMENT(,) = ALL/< Mode Number > SVELOCITY(,) = ALL/< Mode Number > SACCELERATION(,) = ALL/< Mode Number > $ Grid output of real eigenvector for the a-set SVECTOR() = ALL/ $ Grid output of SPC forces SPCFORCES(,) = ALL/ $ Element output of force, stress and strain ELFORCE(,) = ALL/ ELSTRESS(,) = ALL/ STRAIN(,) = ALL/ $ Analysis Cards SPC = < ID of SPC Cards Defined in Bulk Data > METHOD = < ID IN EIGRL > TSTEP = < ID IN TSTEP > $ XY plot output OUTPUT(XYPLOT) XYPUNCH RESPONSE /() XYPUNCH RESPONSE /() XYPUNCH RESPONSE /() $ BULK DATA TSTEP ID Number of Steps, N1 Time Step, ∆t1 Output Every NO1 Steps Number of Steps, N2 Time Step, ∆t2 Output Every NO2 Steps … etc … The integration time step must be small enough to represent accurately both the variation in the loading and also to represent the maximum frequency of interest. If a loading has a frequency content of 500 Hz then the time step should be less than 1/500 s. A very high frequency transient excitation will have very sharp spikes (i.e. very low period). It is necessary for the integration time step to subdivide this. Another reason is the fact that the solution algorithm smoothes the force by taking the average of 3 times steps. Hence, it is important to avoid defining 437 Structural Engineering Analysis and Design Second Edition discontinuous forcing functions. If the analysis calls for sharp impulses, it is best to smooth the impulse over at least one integration time step. It is also recommended to use at least 10 solution time steps per period of response for the cut-off maximum frequency of interest. Hence if the highest frequency of interest is 500 Hz, then the time step should be 1/(500x10) or smaller. Since the solution algorithm is an implicit time integration scheme, the size of the time step is limited for accuracy purposes and not for the stability of the scheme, which becomes the governing criteria in explicit time integration schemes. Since the numerical integration is performed on a small number (as not all the modes are usually included) of uncoupled equations, there is not a large computational penalty for changing ∆t as there is in direct transient response analysis. A constant ∆t is still recommended because an artificial spike occurs each time ∆T is changed, especially if NOLINi is present. As for the duration of analysis, it is important that it be long enough such that the lowest flexible mode oscillates at least through one cycle. So if the first fundamental natural frequency is 0.5 Hz, the duration of analysis should be at the least 2.0 s. In both direct and modal transient response analysis, the cost of integration is directly proportional to the number of time steps. If on one hand, a small time step is required to subdivide the smallest period, a long enough duration of analysis is required to properly capture long period response. This is so because in many cases, the peak dynamic response does not occur at the peak value of load nor necessarily during the duration of the loading. A good rule is to always solve for at least one cycle of response for the longest period mode after peak excitation. To specify the optional initial displacement and velocity conditions (note that initial accelerations is assumed to be zero), $ CASE CONTROL SECTION IC = < ID OF TIC > $ BULK DATA TIC SID Grid ID Component Number Initial Displacement Initial Velocity In this LINEAR TIME DOMAIN solution, the static response must be added to the dynamic response if the dynamic analysis is performed about the initial undeflected (by the static loads) state with only the dynamic loads applied, hence causing the dynamic response to be measured relative to the static equilibrium position. Hence, the total response = the dynamic response + the static response to static loads. Time domain dynamic excitation functions should always be applied from the amplitude of 0.0 (and realistically de-ramped to 0.0 as well). This is because inherently, the dynamic excitation function has to be extrapolated within the analysis code to be from 0.0. Hence, that initial jolt should better be representative of reality irrespective of whether load excitations or enforced motion is being applied. Alternatively, in this LINEAR TIME DOMAIN solution, if the dynamic analysis is performed with the deflected static shape as initial input and the static loads maintained throughout the dynamic excitations, the total or absolute response (static and dynamic) is obtained straight away from the dynamic analysis. Hence total response = dynamic response (which already includes the static response to static loads). Of course, if the transient dynamic analysis follows a static analysis (by say SOL 101, SOL 106, implicit dynamic relaxation by SOL 129 or explicit dynamic relaxation), then the dynamic excitation function should be ramped up from the static amplitude and not from 0.0 (and realistically de-ramped to the static load as well), so that again there would be no jolt unrepresentative of reality. 438 Structural Engineering Analysis and Design Second Edition 4.7.6.1.1 Applied Load Excitations Applied load excitations are as described in direct forced transient response analysis. 4.7.6.1.2 Nonlinear Transient Load Nonlinear transient loads are as described in nonlinear forced transient response analysis. 4.7.6.1.3 Enforced Motion Enforced motion is as described in direct forced transient response analysis. 4.7.6.1.4 Damping Viscous and structural modal damping is defined as follows. TYPE refers to the type of damping units, i.e. whether structural damping G (default), critical damping CRIT or quality factor Q. The values of fi and gi define pairs of frequencies and damping. Straight-line interpolation is used for modal frequencies between consecutive fi values. Linear extrapolation is used for modal frequencies outside the entered range. ENDT ends the table input. $ CASE CONTROL SECTION SDAMPING = < ID IN TABDMP1 > $ BULK DATA TABDMP1 ID TYPE f1 g1 f2 g2 f3 g3 f4 f5 g5 f6 g6 … … ENDT g4 Because time domain solutions (be it a modal method or a direct method) cannot handle structural damping, an equivalent viscous damping is required. Hence, if structural damping is specified at the element levels, then the incorrect modal damping will result because the conversion from structural to viscous damping will only be valid for one modal natural frequency, w4 as specified by PARAM, W4 (Note that element viscous damping damps different modes accurately). Hence, if the model has any structural damping, then it should be specified as modal damping. Modal damping can be calculated using SOL 107 and specified as either modal structural or modal viscous damping (hence a modal method of analysis i.e. SOL 112 must be used). Of course, the modal damping will be converted to modal viscous damping for solution in the time domain. This conversion is only perfectly accurate when the frequency of excitation matches the natural frequency of the mode (at resonance), but of course this is acceptable as only that is the instance when the damping estimate is most critical. Note that in the frequency domain, for the modal solution (SOL 111), the modal damping specified will be converted to either modal viscous or modal structural damping depending on PARAM, KDAMP. 439 Structural Engineering Analysis and Design Second Edition 4.7.6.2 GL, ML P-∆ (KGA From KEA) Modal Forced Transient Response Analysis It is often necessary to incorporate the reduction in bending stiffness of gravity load resisting columns for the analysis of lateral loads. The following procedure is undertaken. Phase 1 Perform static analysis (with loads that cause the greatest negative or positive geometric stiffness) based on [KEA] but include the segyroa.v2001 alter prior to the Case Control Section in order to compute the geometric stiffness matrix [KGA]1 (and output into a .pch file) based on the generated element loads from the [KEA] static analysis. Phase 2 A SOL 112 with a general loading function is undertaken based on [KEA] + [KGA]1 with the k2gg=ktjj statement in the Case Control Section and the outputted .pch file which contains the ktjj matrix in the Bulk Data. The responses at this stage represent the P-∆ (KGA From KEA) response to the dynamic excitation. The following equivalent alternative procedure can also be employed. $ CASE CONTROL SECTION SUBCASE 1 LABEL = Static Preload Load Case LOAD = < ID of FORCEi, MOMENTi, PLOADi, GRAV, LOAD, SPCD Cards in Bulk Data > TEMP(LOAD) = < ID of TEMP, TEMPRB, TEMPP1 Cards in Bulk Data > DEFORM = < ID of DEFORM Cards in Bulk Data > SUBCASE 2 LABEL = P-∆ Modal Transient Response Analysis STATSUB(PRELOAD) = 1 DLOAD = < ID OF TLOAD1 or TLOAD2 > The method is valid when only the prestress is judged to affect the geometric stiffness such as in the compressive preload of building columns due to gravitational loads and the prestressing of extremely taut cables that sag very little under gravity but not in systems such as suspension bridges. Where lateral loads are large enough to affect the geometry of the system with prestress, then a repetitive P-∆, SOL 106, implicit dynamic relaxation SOL 129 or explicit dynamic relaxation must be employed. But in single P-∆ analysis, because cables do not have much elastic bending stiffness, the initial static preload subcase should only include the prestress and not gravity as including gravity is the same as solving two linear static problems of stiffness KEA with preload and gravity as the applied loads respectively. Clearly, in the gravity case, it is nonsensical as the cables do in reality have differential stiffness (from the prestress) to resist the gravitational force. Prestress in one direction (i.e. along the axis of cable) will cause a differential stiffness in the orthogonal direction. Gravity acts in the orthogonal direction and hence cannot be accounted for in the calculation of the prestress in this single P-∆ analysis. To quantitatively decide if gravity need not be considered in contributing to the differential stiffness of the cables, a static P-∆ analysis should be carried out, the first subcase being a SOL 101 with only the prestress as applied loads and the second subcase a P-∆ SOL 101 (i.e. utilizing the induced prestress from the first subcase to form a geometric stiffness matrix) with both the gravity and prestress included as applied loads. If the difference in the cable element forces between subcases 1 and 2 is negligible, then gravity has little influence in affecting the geometric stiffness. If there is a major difference in the cable element force, then clearly, gravity will affect the geometric stiffness and as such, a repetitive P-∆ , SOL 106, implicit dynamic relaxation or explicit dynamic relaxation must be used to converge to the true KT. Likewise, in the single P-∆ analysis of multi-storey buildings, gravity (and only gravity) acts in axis of columns to generate prestress, and the differential stiffness is computed for the orthogonal direction reducing resistance to lateral wind forces, applied in the second subcase with gravity too. 440 Structural Engineering Analysis and Design Second Edition When a static subcase is specified for linear transient response analysis (SOLs 109 and 112) with STATSUB(PRELOAD), the data recovery is controlled by PARAM, ADSTAT. By default (YES) the static solution will be superimposed on the dynamic response solution (displacement, stress and SPCForce). The relative solution can be obtained in reference to the static solution point by PARAM, ADSTAT, NO. No provision is made for frequency response analysis, because the static responses contribute only to the zero frequency response. For linear dynamic response, the static solution can be superimposed after the dynamic solution procedure. The preload effect is reflected only in the stiffness and the actual static load is omitted in the dynamic response analysis. The total displacement can be obtained by superposing the static solution to the transient response analysis. And the stress output is obtained as The STATSUB(PRELOAD) computes the differential stiffness due to the prestress and also the follower force. The follower force is calculated and incorporated by the use of PARAM, FOLLOWK, YES. We know how the prestress affects the differential stiffness, namely a tensile prestress causing an increase in stiffness. The effect of the follower force on the stiffness is different. For example, for a cylinder under external pressure critical buckling load may be overestimated (even though the mode shapes are similar) in a SOL 105 and the natural frequencies in vibration may be underestimated (even though the mode shapes are similar) in a SOL 103 in the absence of follower stiffness. To the contrary, these observations are reversed in case of centrifugal loads. Centrifugal forces as a constant (static) load are applied by a Bulk Data RFORCE to any elements that have masses. The follower stiffness due to centrifugal load has the effect of lowering stiffness (although the centrifugal load tensioning effect increases stiffness), consequently lowering natural frequencies (even though the mode shapes are similar) in a SOL 103 and lowering the buckling loads (even though the mode shapes are similar) in a SOL 105. This effect increases as the RPM increases, and it becomes significant when the RPM is over 1000. For moderately geometric nonlinear analysis, exclusion of follower stiffness affects the rate of convergence, but the converged solution is correct. For severely geometric nonlinear analysis, it may not be possible to obtain a converged solution without including follower stiffness. As the geometric nonlinearity intensifies, so is the effect of follower stiffness. Therefore, inclusion of follower stiffness greatly enhances the convergence if the deformation involves severe geometric nonlinearity. 441 Structural Engineering Analysis and Design Second Edition 4.7.6.3 GL, ML P-∆ (KGA From Exact or Approximate KTA) Modal Forced Transient Response Analysis It is often necessary to include the differential stiffness, especially if there are prestressed cables in the model. To obtain KTA, to be theoretically exact, a GNL SOL 106 (or implicit dynamic relaxation SOL 129 or explicit dynamic relaxation LS-DYNA) with prestress (as temperature loads say) and gravity must be undertaken. Alternatively, an approximation to KTA can be obtained by repetitive P-∆ static analyses with the prestress (as temperature loads say) and gravity applied. The procedure to obtain this approximate KTA will be presented. Note that the approximate KTA will be the summation of the elastic stiffness KE at the undeflected (by the prestress and gravity) state but KG at the deflected (by the prestress and gravity) state. Hence if KE changes considerably during the application of the prestress, a full SOL 106 (or implicit dynamic relaxation SOL 129 or explicit dynamic relaxation LS-DYNA), which converges to the KE and KG at the deflected (by the prestress and gravity) state should be employed. Hence for the modelling of a suspension bridge where there is a great change in geometry (known in the bridge industry as form-finding, so-called because it is necessary to find the form or shape of the catenary suspension cables), it may be prudent to employ SOL 106 (or implicit dynamic relaxation SOL 129 or explicit dynamic relaxation LSDYNA), but for a high tension low sag cable on say a tower with prestressed cables, the repetitive P-∆ static analysis may be adequate. The repetitive P-∆ analysis basically involves a number of iterations of linear static analyses to obtain an approximate KTA. Note again that A refers to the initial undeflected (by the collapsing load) state, but deflected by the prestress and gravity. To perform the repetitive P-∆ analysis, a static analysis is performed based on KEA with temperature loads and gravity to generate forces in the structural elements, which in turn provides input for the computation of KGiAKTm where m is the iterations. Repetitive static analysis is performed with the prestress and gravity updating the stiffness matrix KEA + KGiAKTm-1 + KGiAKTm until convergence of displacements is obtained. The tangent stiffness at this stage is the approximate converged tangent stiffness matrix KTA = KEA + KGiAKT. The converged displacements represent the approximate P-∆ (KGA From Approximate KTA) static response to the initial prestress loads. The converged geometric stiffness at this stage would be that based upon the approximate tangent stiffness matrix KTA, i.e. KGiAKT. Phase 1 Perform static analysis (with prestress and gravity) based on [KEA] but include the segyroa.v2001 alter prior to the Case Control Section in order to compute the geometric stiffness matrix [KGA]1 (and output into a .pch file) based on the generated element loads from the [KEA] static analysis. Phase 2 Perform static analysis (with prestress and gravity) based on [KEA] + [KGA]1 by including the k2gg = ktjj statement in the Case Control Section, the outputted .pch file which contains the ktjj matrix in the Bulk Data and the segyroa.v2001 alter prior to the Case Control Section to compute the [KGA]2 (and output into the .pch file overwriting previous data) based on the generated element loads from the [KEA] + [KGA]1 static analysis. Phase 3 Repeatedly perform the Phase 2 static analysis (with prestress and gravity) based on [KEA] + [KGA]i for i = 2 to n where n represents the number of iterations required for the change in deflections between analyses to become negligible. This would signify that the change in the [KGA] matrix become negligible and the correct [KGA] is attained. The deflections and the other responses at this stage represent the P-∆ (KGA From Approximate KTA) static response to the prestress and gravity. The stiffness of the structure is KTA. Phase 4 A SOL 112 with a general loading function is undertaken with the k2gg=ktjj statement in the Case Control Section and the outputted .pch file which contains the latest ktjj matrix in the Bulk Data. The responses at this stage represent the P-∆ (KGA From Approximate KTA) response to the dynamic excitation. 442 Structural Engineering Analysis and Design Second Edition 4.7.7 4.7.7.1 Hand Methods Verification Determination of Maximum Dynamic Displacement for Deterministic Time Domain Loading by Transforming the Coupled MDOF Linear Undamped ODEs To a Set of Independent (Uncoupled) SDOF ODEs and Solving the Independent Equations in a Manner Similar to Solving a SDOF ODE Linear time domain hand methods are capable of analyzing: - Multi-Modal Response to Deterministic Non-Periodic Short Duration Impulse and Hence Random Non-Stationary Short Duration Impulse by Enveloping Deterministic Responses A coupled MDOF system of linear ODEs must be uncoupled to a set of independent SDOF system of linear ODEs if any feasible hand method computation is to be employed. These independent SDOF ODEs can be solved using standard techniques of solving SDOF linear dynamic ODEs. The final stage to the analysis is to employ a modal superposition method to express the total response as a summation of the results from the solution of the individual modal equations. Note that since the modal frequencies and the corresponding mode shapes are required to uncouple the coupled MDOF ODEs, the real eigenvalue analysis must be performed first. It was shown that a system of coupled MDOF ODEs could be reduced to a system of independent SDOF ODEs by employing the orthogonality properties of real modes Mi & ξ&i ( t ) + C i ξ&i ( t ) + K i ξ i ( t ) = Pi (t) for the i th mode where the generalized (or modal) terms are obtained from solving the real eigenvalue problem M i = {φ i } [M ]{φ i } T C i = ζ i 2M i ω n i K i = {φ i } [K ]{φ i } = ω 2ni M i T Pi (t) = {φ i } {P( t )} T The modal properties (i.e. modal masses, modal frequencies and hence modal stiffness) can be obtained by performing a real modal analysis SOL 103 and if required the modal damping can also be incorporated from a complex modal analysis SOL 107. The normalization of the mode shapes can be arbitrary. The normalization technique employed will not affect the value of the modal frequencies but of course will determine the values of the modal masses (and hence modal damping and stiffnesses) and the (amplitude of the) modal force. Although the normalization technique is arbitrary, it is recommended that the normalization employed would facilitate the calculation of the (amplitude of the) modal force since this is a hand calculation. To facilitate the computation, it is wise to choose the normalization to be unity at the DOF of application of the external excitation. Either way, the modal force (for a particular mode) for discrete loading points is calculated as follows Pi (t) = {φ i } {P( t )} T Had the loading been continuous, a continuous modal force can also be calculated by hand (or a spreadsheet) as follows L Pi (t) = ∫ φ i ( x ){P( x , t )}dx 0 There will be n uncoupled ODEs for n natural modes. These are now simply SDOF ODEs, which can be solved using Duhamel’s integral. For a particular mode i, for a general loading function Pi(t), from SDOF response analysis, we can establish Di(t) Dimax = = dynamic amplification factor in the time domain maximum dynamic amplification factor in the time domain 443 Structural Engineering Analysis and Design Second Edition Note that in general, Di(t) is a function of the natural circular frequency ωni2 = Ki/Mi or the damped natural circular frequency ωd, the time duration of loading td and the general time t. Dimax is a function of the natural circular frequency ωni2 = Ki/Mi or the damped natural circular frequency ωd and the time duration of loading td. From this, we can establish the modal responses ξi(t) ξimax = = modal displacement response (in modal space) in the time domain, Di(t)(p0i/ Ki) maximum modal displacement response in the time domain, Dimax(p0i/ Ki) Note that p0i corresponds to the amplitude of the modal loading function Pi(t) and not simply the amplitude of the loading function {P(t)}, i.e. p0 at any particular node. Of course, if the normalization of the mode was such that it was unity at the DOF of application of the external force with amplitude p0 then, p0i will be equal to p0. The dynamic amplification factor can be derived for standard short duration loadings as follows. Excitation An Instantaneous Continuous Constant Force of Amplitude p0 An Instantaneous Rectangular Force of Duration td and of Amplitude p0 An Instantaneous Right Angled Triangular Force of Duration td and of Amplitude p0 Undamped (Unless Specified Otherwise) Dynamic Amplification Factor of Mode i, Di (t) Di (t) = 1 – cos ωnt An Instantaneous Isosceles Triangular Force of Duration td and of Amplitude p0 τ < td D i ( t ) = (1 − cos ω n t ) + 1 td τ < td Dimax = 2    τ > td D i max = 2 sin ω n  sin ω n t   − t   ω n   1 τ > td D i ( t ) = (sin ω n t − sin ω n (t − t d )) − cos ω n t ωn t τ < td D i ( t ) = td 2 Plot Di (t) versus td/T to determine maximum response 2 (ω n t − sin ω n t ) ωn t d td/2 < τ < td D i ( t ) = τ > td D i ( t ) = An Instantaneous Half Sine Force of Frequency ω and of Amplitude p0 Dimax = 2 τ < td Di (t) = 1 – cos ωnt 2t − t d −t  τ > td D i ( t ) =  − 2 sin ω n sin ω n d 2 2  τ < td/2 D i ( t ) = Undamped (Unless Specified Otherwise) Maximum Dynamic Amplification Factor of Mode i, Dimax 2 [ω n (t d − t ) + 2 sin ω n (t − t d / 2) − sin ω n t ] ωn t d Plot Di (t) versus td/T to determine maximum response 2 [2 sin ωn (t − t d / 2) − sin ωn t − sin ωn (t − t d )] ωn t d 1 (1 − ω τ > td D i ( t ) = − 2 / ω2n )   ω  sin ωt − sin ωn t   ω n   ω / ωn (1 − ω 2 / ω2n ) (sin ω t + sin ω (t − t n n d )) Plot Di (t) versus td/T to determine maximum response The above table shows that the maximum dynamic amplification that can be produced is two times the static displacement! This occurs for the instantaneous applied continuous constant force. The response spectrum showing the maximum responses from plots of Di(t) versus td/Ti for various td/Ti is presented. 444 Structural Engineering Analysis and Design Second Edition Response Spectrum 2.5 2 Dimax 1.5 1 0.5 0 0 0.5 1 1.5 2 2.5 3 3.5 4 4.5 td/T i The response from an impulse is even easier to obtain as the unit impulse function can be brought outside the integral (i.e. the Duhamel’s or Convolution Integral). The maximum modal response (in modal space) from an impulse (t1/T < 0.2), can be obtained simply as follows. ∫ ξ i (τ = t ) = h(t - τ) ξ i max = 1 M i ω ni ξ i max = 1 M i ω di ∫ τ= t τ= 0 ∫ τ= t τ= 0 τ= t τ= 0 p( τ)dτ φ i p(τ)dτ undamped φ i p(τ)dτ damped where φ i = mod al component at excitation point The above expression may seem to differ from the dynamic amplification approach where the denominator contains the modal stiffness, i.e. modal mass times the square of the natural circular frequency. This is because the above expression requires the explicit integration of the forcing function. The dynamic amplification approach differs in the sense that the integral (i.e. Duhamel’s Integral) is already classically integrated to obtain the expression D(t). Another equivalent interpretation of the above relationship is from the basic consideration of the conservation of momentum. The impacting particle (of small relative mass compared to mass of structure) imposes an impulse I onto the structure. The magnitude of I can be calculated as m∆v where m is the small mass and ∆v the change of velocity at impact. If there is no rebound ∆v is the approach velocity. Conservation of momentum at impact requires the initial velocity of the structural mass to be I/M. A lightly damped system then displays damped free vibration with an initial displacement of approximately I/(ωdM), or an initial velocity of approximately I/M or an initial acceleration of approximately Iωd/M. And the modal response (in modal space) from a general loading function that cannot be classically integrated can be obtained by employing a numerical integration technique such as Simpson’s Rule. ξ i (τ = t ) = 1 M i ω ni = sin ω ni t ∫ τ= t τ= 0 φ i p(τ) sin ω ni ( t − τ)dτ 1 M i ω ni ∫ τ= t τ= 0 φ i p(τ) cos ω ni τdτ − cos ω ni t 445 1 M i ω ni ∫ τ= t τ= 0 φ i p(τ) sin ω ni τdτ Structural Engineering Analysis and Design Second Edition Once the individual modal responses {ξ(t)} are computed, the physical response can be calculated from {u(t)} = [Φ ]{ξ( t )} For a 2 DOF system, this expression would be  u1 ( t )   φ11  = u 2 ( t )  φ 21 φ12   ξ1 ( t )    φ 22  ξ 2 ( t ) The above computation takes into account the phase difference between the responses of different modes. It is important to point out that the maximum of the modal responses do not occur at the same time. As shown above, the exact solution can be obtained by expanding the general u(t) expression to include all the modes considered, and only then maximised. However, this may prove to be mathematically involved if differentiation is to be performed analytically by hand (the computerized method of course performs the response calculation at discrete time points as it is not just the maximum that is of interest). An alternative would be to instead of maximising the physical response, maximise the modal responses and then only superpose the modal responses for the physical response. This is equivalent to the response spectrum method (only that the procedure is employed on a deterministic loading function instead of a random function). The square root of sum of squares (SRSS) of the maximum modal contributions as follows, depicted for a 2 DOF dynamic system.  u 1 max   (φ11ξ1 max )2 + (φ12 ξ 2 max )2   =  u 2 max   (φ 21ξ1 max )2 + (φ 22 ξ 2 max )2  If the modal natural frequencies are too close to each other (within about 10%), then the Complete Quadratic Combination (CQC), which is based on random vibration theory should be used. These methods of approximating the maximum multi-modal responses are effectively response spectrum analyses on a deterministic loading function (as opposed to a non-stationary random loading function which is normally associated with response spectrum analysis). The upper limit would be to choose all the eigenvectors to have the maximum modal response at the same time. This is obtained by multiplying the moduli as follows. {u ( t )} = [Φ ] {ξ i max } Often, we need to ascertain other types of response. The modal velocities and accelerations can easily be obtained by differentiating the {ξ(t)} vector with respect to time t and hence, {u&( t )} = [Φ ]{ξ&( t )} {& u&( t )} = [Φ ]{& ξ&( t )} Finally, the SRSS superposition, again depicted for the 2 DOF system, u&1 ( t )   φ11 φ12  & & ξ&1 ( t )   = &   u&2 ( t ) φ 21 φ 22  ξ&2 ( t ) & ( ( u&1max   φ11& & ξ&1max ∴ = u&2 max   φ & & &  21ξ1max ) + (φ ) + (φ & & 2 12 ξ 2 max 2 22 ξ 2 max & & )   )  2 2 446 Structural Engineering Analysis and Design Second Edition For whatever response be it the displacement, velocity acceleration or force, the individual modal responses should first be calculated in terms of time t, then maximised, then only combined for the physical response with some method of superposition. Do not maximise the modal displacement response and base the other responses on that. It must be understood that the scaling (or normalization) of the normal modes are arbitrary, hence their do not indicate the response. This means that a different scaling method will yield a different modal (or generalized) mass, modal stiffness (but same modal frequency) and (amplitude of) modal force. It follows that the modal response ξi(t) from a particular mode will be not be unique and will be dependent upon how the eigenvectors are scaled. However, the response in the physical coordinates for each and every mode will be unique irrespective of how the eigenvectors are scaled. This can be proven just by studying the modal equations above. The equation of dynamic equilibrium for a mode is given by Mi & ξ&i ( t ) + K i ξ i ( t ) = Pi (t) T T {φi }T [M]{φi }& ξ&i ( t ) + {φ i } [K ]{φ i }ξ i ( t ) = {φi } {P( t )} It is evident that for each mode i, the modal mass Mi, modal stiffness Ki and the amplitude of the modal force p0i is all dependent upon an arbitrarily scaled eigenvector. The modal frequency ωni2 = Ki/Mi on the other hand is unique to the mode. It follows that the maximum dynamic amplification factor Dimax is also unique to the mode since it is a function of the natural circular frequency ωni2 = Ki/Mi and the time duration of loading td. However, the maximum modal displacement response, ξimax = Dimax(p0i/ Ki) is dependent upon the scaling of the eigenvector. The response in the physical coordinates {uimax} = {φi}ξimax. Say an eigenvector was to be arbitrarily scaled up by say 3. Hence, New Mi New Ki New ωni2 New Dimax New ξimax New {uimax} = 9Mi = 9 Ki = ωni2 = Dimax = Dimax 3p0i / (9Ki) = Dimax p0i / (3Ki) = 3{φi} ξimax = 3{φi} Dimax p0i / (3Ki) = {φi} Dimax p0i / Ki = {uimax} as before As a final note, if the eigenvector i was scaled such that its component is unity at the DOF which corresponds to both the solitary point of application of load and the response, then {u i max }response point of interest = {φ i }response point of interest ξ i max {u i max }response point of interest = 1.0ξ imax As eigenvector term unity at point of interest {φ i }response point of interest = 1.0 = 1.0D imaxp 0i Ki As eigenvector term unity at solitary point of application of load p 0i = 1.0p 0 {u i max }response point of interest = 1.0D i max 1.0p 0 Ki = D i max p 0 Ki = D i max p 0 ω2niMi Since K i = ω2niMi {u i max }response point of interest 447 Structural Engineering Analysis and Design Second Edition The significance of this result is that if the eigenvector i was scaled such that its component is unity at the DOF which corresponds to both the solitary point of application of load and the response, the physical response due to the particular mode can be seen to be just proportional to the dynamic amplification Dimax (which is a function of the excitation frequency and the natural frequency ωni) and the amplitude of the loading function p0, and inversely proportional to square of the natural frequency ωni and the modal mass Mi. The dynamic displacement response is then basically the static deflection scaled by the maximum dynamic amplification factor. Another important significance is that with this normalization technique applied to all the modes, the relative importance of different modes to a certain force excitation at a certain location can be determined. That is to say, if all the eigenvectors were scaled such that its component is unity at the DOF which corresponds to both the solitary point of application of load and the response (using POINT normalization), then the greater the modal mass, the less important is the mode as the response is inversely proportional to the modal mass. Unlike natural frequencies, the relative importance of modes is not a structural property. It is dependent upon the location of the excitation force and the location of the response. 448 Structural Engineering Analysis and Design Second Edition A forced response analysis of a shear frame (be it to model a building or water tank) connected by a mass-less flexible beam is illustrated in MAPLE 7. All units in SI. u2 u1 L P(t) 6EI/L3 M EI EI P(t) M L EI EI EI = 560000000 M = 400000 L=4 100000 0.64 t System and Frequency Domain Excitation Description - User Input > restart; with(LinearAlgebra): DOF:=2: EI:=560000000: M:=400000: L:=4: MASS:=Matrix([[M,0],[0,M]]); KE:=Matrix([[30*EI/L^3,-6*EI/L^3],[-6*EI/L^3,30*EI/L^3]]); # Excitation - Po is the amplitude of the excitation, i.e. P(t)=Po*function of t P(t):=Matrix([[0],[100000]]); td:=0.64; 0 400000 MASS :=    0 400000   262500000 -52500000 KE :=   -52500000 262500000   0  P( t ) :=  100000   td := .64 Modal Properties of System - Solution of Real Eigenvalue Problem [K-λM]{φ}={0} - Note that Eigensolution may not arrange the roots sequentially - MAX normalization of the Eigenvectors > Eigensolution:=Eigenvectors(MatrixInverse(MASS).KE): lambda:=Matrix(Eigensolution[1],shape=diagonal): wn:=map(sqrt,evalf(lambda)); Phi:=Eigensolution[2]; for j from 1 to DOF do eig:=0: for i from 1 to DOF do eig:=eig,Phi[i,j]; end do; for i from 1 to DOF do Phi[i,j]:=Phi[i,j]/max(eig); end do; end do: 449 Structural Engineering Analysis and Design Second Edition Phi:=Phi; 0.  22.91287847 wn :=    0. 28.06243040   1 Φ :=  1  -1  1 1 Φ :=  1  -1  1 Uncoupling The Equations of Motion > MODALMASS:=evalf(Transpose(Phi).MASS.Phi); MODALSTIFFNESS:=evalf(Transpose(Phi).KE.Phi); MODALFORCE:=evalf(Transpose(Phi).P(t)); 0.  800000. MODALMASS :=    0. 800000.  .420000000 10 MODALSTIFFNESS :=   0.  9 0.   .630000000 109 100000. MODALFORCE :=  100000.   Modal Responses ξi = Di(t)Poi/Ki > D(t):=Vector(DOF): for i from 1 to DOF do D(t)[i]:=1-cos(wn[i,i]*t)+1/td*(sin(wn[i,i]*t)/wn[i,i]-t); end do; variablelegend:=seq(convert(D[i],string),i=1..DOF): plot([seq(D(t)[i],i=1..DOF)], t=0..td, D,title="Dynamic Magnification D(t)", legend=[variablelegend]); xi:=Vector(DOF): for i from 1 to DOF do xi[i]:=D(t)[i]*MODALFORCE[i,1]/MODALSTIFFNESS[i,i]; end do: xi:=evalf(xi); D( t ) := 1 − cos ( 22.91287847t ) + .06819309072 sin ( 22.91287847t ) − 1.562500000t 1 D( t ) := 1 − cos ( 28.06243040 t ) + .05567942541 sin( 28.06243040 t ) − 1.562500000 t 2 ξ := [ .0002380952381− .0002380952381 cos ( 22.91287847 t ) + .00001623645017sin( 22.91287847 t ) − .0003720238095 t ] [ .0001587301587− .0001587301587 cos ( 28.06243040 t ) + .883800403210-5 sin( 28.06243040 t ) − .0002480158730 t ] Physical Response in Time Domain > u(t):=Vector(DOF): u(t):=Phi.xi; 450 Structural Engineering Analysis and Design Second Edition u( t ) := [ .0000793650794− .0002380952381 cos ( 22.91287847t ) + .00001623645017sin( 22.91287847t ) − .0001240079365t + .0001587301587 cos ( 28.06243040t ) − .883800403210-5 sin( 28.06243040t ) ] [ .0003968253968− .0002380952381 cos ( 22.91287847t ) + .00001623645017sin( 22.91287847t ) − .0006200396825t − .0001587301587 cos ( 28.06243040t ) + .883800403210-5 sin( 28.06243040t ) ] Plot of Response in Time Domain > variablelegend:=seq(convert(u[i],string),i=1..DOF): plot([seq(u(t)[i],i=1..DOF)], t=0..td, Displacement,title="Steady-State Displacement Response", legend=[variablelegend]); 451 Structural Engineering Analysis and Design Second Edition 4.7.7.2 Determination of Max Dynamic Displacement for Deterministic Time Domain Support Motion (Displacement, Velocity or Acceleration) by Transforming the Coupled MDOF Linear Undamped ODEs (In Relative Terms) To a Set of Independent (Uncoupled) SDOF ODEs (In Relative Terms) and Solving the Independent Equations in a Manner Similar to Solving a SDOF ODE Linear time domain hand methods are capable of analyzing: - Multi-Modal Response to Deterministic Non-Periodic Short Duration Impulse Enforced Motion and Hence Random Non-Stationary Short Duration Impulse Enforced Motion by Enveloping Deterministic Responses For a MDOF system, the equation of motion for support excitation in relative terms is [M ]{& u&( t )} + [C]{u&( t )} + [K ]{u ( t )} = −[M ]{1}& u&s ( t ) Note that {D} = {1} is a unity vector corresponding to the rigid body motion. The support excitation causes all the masses to produce an inertial force opposing its motion (D’Alembert’s Principle). This coupled MDOF system could be reduced to a system of independent SDOF ODEs by employing the orthogonality properties of real modes Mi & ξ&i ( t ) + C i ξ&i ( t ) + K i ξ i ( t ) = Pi (t) for the i th mode where the generalized (or modal) terms are obtained from solving the real eigenvalue problem M i = {φ i }T [M ]{φ i } C i = ζ i 2M i ω n i K i = {φ i } [K ]{φ i } = ω 2ni M i T Pi (t) = −{φ i }T [M ]{1}& u&s ( t ) The modal properties (i.e. modal masses, modal frequencies and hence modal stiffness) can be obtained by performing a real modal analysis SOL 103 and if required the modal damping can also be incorporated from a complex modal analysis SOL 107. The normalization of the mode shapes can be arbitrary. The normalization technique employed will not affect the value of the modal frequencies but of course will determine the values of the modal masses (and hence modal damping and stiffnesses) and the (amplitude of the) modal force. Note that the modal force (for a particular mode) for discrete loading points is calculated as follows Pi (t) = −{φ i } [M ]{1}& u&s ( t ) T There will be n uncoupled ODEs for n natural modes. These are now simply SDOF ODEs, which can be solved using Duhamel’s integral. T Mi& ξ&i ( t ) + C i ξ&i ( t ) + K i ξ i ( t ) = −{φ i } [M ]{1}& u&s ( t ) For a particular mode i, for a general loading function Pi(t), from SDOF response analysis, we can establish Di(t) Dimax = = dynamic amplification factor in the time domain maximum dynamic amplification factor in the time domain Note that in general, Di(t) is a function of the natural circular frequency ωni2 = Ki/Mi or the damped natural circular frequency ωd, the time duration of loading td and the general time t. Dimax is a function of the natural circular frequency ωni2 = Ki/Mi or the damped natural circular frequency ωd and the time duration of loading td. From this, we can establish the modal responses 452 Structural Engineering Analysis and Design Second Edition p 0i {φ }T [M ]{1}& u&0 & = − D i (t ) i 2 u&0 = amplitude Ki ω ni M i Thus whereby we had the following for the modal response in load excitations ξ i ( t ) = D i (t ) {φ } {p } p ξ i ( t ) = D i ( t ) 0i = D i ( t ) i 2 0 Ki ω ni M i T we now have the following for enforced base motion ξ i (t) = D i (t) p 0i {φ }T [M ]{1}& u&0 = −D i (t) i 2 Ki ω ni M i An interesting observation is that whereby for load excitations the amplitude of the forcing vector {p0} may be sparse with only possibly one point with a value, that for enforced motion is quite different [M]{1} & u&0 with all components having a value. Let us also define the modal participation factor for enforced motion as Γi = − {φ i }T [M]{1} Mi =− {φ i }T [M]{1} {φ i }T [M]{φ i } Hence, the modal response for enforced motion excitations ξ i ( t ) = D i (t )Γi & u&0 ω 2ni The dynamic amplification factor can be derived for standard short duration loadings as follows. Excitation An Instantaneous Continuous Constant Force of Amplitude p0 An Instantaneous Rectangular Force of Duration td and of Amplitude p0 An Instantaneous Right Angled Triangular Force of Duration td and of Amplitude p0 Undamped (Unless Specified Otherwise) Dynamic Amplification Factor of Mode i, Di (t) Di (t) = 1 – cos ωnt An Instantaneous Isosceles Triangular Force of Duration td and of Amplitude p0 2t − t d −t  τ > td D i ( t ) =  − 2 sin ω n sin ω n d 2 2  τ < td D i ( t ) = (1 − cos ω n t ) + 1 td τ < td Dimax = 2    τ > td D i max = 2 sin ω n  sin ω n t   − t   ω n   1 τ > td D i ( t ) = (sin ω n t − sin ω n (t − t d )) − cos ω n t ωn t τ < td D i ( t ) = td 2 Plot Di (t) versus td/T to determine maximum response 2 (ω n t − sin ω n t ) ωn t d td/2 < τ < td D i ( t ) = τ > td D i ( t ) = An Instantaneous Half Sine Force of Frequency ω and of Amplitude p0 Dimax = 2 τ < td Di (t) = 1 – cos ωnt τ < td/2 D i ( t ) = Undamped (Unless Specified Otherwise) Maximum Dynamic Amplification Factor of Mode i, Dimax 2 [ω n (t d − t ) + 2 sin ω n (t − t d / 2) − sin ω n t ] ωn t d Plot Di (t) versus td/T to determine maximum response 2 [2 sin ωn (t − t d / 2) − sin ωn t − sin ωn (t − t d )] ωn t d 1 (1 − ω τ > td D i ( t ) = − 2 / ω2n )   ω  sin ωt − sin ωn t   ωn   ω / ωn (1 − ω 2 / ω2n ) (sin ω t + sin ω (t − t n 453 n d )) Plot Di (t) versus td/T to determine maximum response Structural Engineering Analysis and Design Second Edition The above table shows that the maximum dynamic amplification that can be produced is two times the static displacement! This occurs for the instantaneous applied continuous constant force. The response spectrum showing the maximum responses from plots of Di(t) versus td/Ti for various td/Ti is presented. Response Spectrum 2.5 2 Dimax 1.5 1 0.5 0 0 0.5 1 1.5 2 2.5 3 3.5 4 4.5 td/T i Once the individual modal responses {ξ(t)} are computed, the physical response can be calculated from {u(t)} = [Φ ]{ξ( t )} For a 2 DOF system, this expression would be  u1 ( t )   φ11  = u 2 ( t )  φ 21 φ12   ξ1 ( t )    φ 22  ξ 2 ( t ) The above computation takes into account the phase difference between the responses of different modes. It is important to point out that the maximum of the modal responses do not occur at the same time. As shown above, the exact solution can be obtained by expanding the general u(t) expression to include all the modes considered, and only then maximised. However, this may prove to be mathematically involved if differentiation is to be performed analytically by hand (the computerized method of course performs the response calculation at discrete time points as it is not just the maximum that is of interest). An alternative would be to instead of maximising the physical response, maximise the modal responses and then only superpose the modal responses for the physical response. This is equivalent to the response spectrum method (only that the procedure is employed on a deterministic loading function instead of a random function). The square root of sum of squares (SRSS) of the maximum modal contributions as follows, depicted for a 2 DOF dynamic system.  u 1 max   (φ11ξ1 max )2 + (φ12 ξ 2 max )2   =  u 2 max   (φ 21ξ1 max )2 + (φ 22 ξ 2 max )2  If the modal natural frequencies are too close to each other (within about 10%), then the Complete Quadratic Combination (CQC), which is based on random vibration theory should be used. These methods of approximating the maximum multi-modal responses are effectively response spectrum analyses on a deterministic loading 454 Structural Engineering Analysis and Design Second Edition function (as opposed to a non-stationary random loading function which is normally associated with response spectrum analysis). The upper limit would be to choose all the eigenvectors to have the maximum modal response at the same time. This is obtained by multiplying the moduli as follows. {u ( t )} = [Φ ] {ξ i max } Often, we need to ascertain other types of response. The modal velocities and accelerations can easily be obtained by differentiating the {ξ(t)} vector with respect to time t and hence, {u&( t )} = [Φ ]{ξ&( t )} {& u&( t )} = [Φ ]{& ξ&( t )} Finally, the SRSS superposition, again depicted for the 2 DOF system, u&1 ( t )   φ11 φ12  & & ξ&1 ( t )   = &   u&2 ( t ) φ 21 φ 22  ξ&2 ( t ) & ( ( u&   φ & & ξ& ∴  1max  =  11 1max u&2 max   φ & & &  21ξ1max ) + (φ ) + (φ & & 2 12 ξ 2 max 2 22 ξ 2 max & & )   )  2 2 For whatever response be it the displacement, velocity acceleration or force, the individual modal responses should first be calculated in terms of time t, then maximised, then only combined for the physical response with some method of superposition. Do not maximise the modal displacement response and base the other responses on that. 455 Structural Engineering Analysis and Design Second Edition 4.7.7.3 Determination of Maximum Dynamic Displacement for Deterministic Time Domain Loading by Transforming the Coupled Distributed System Linear Damped ODEs (from the governing PDE) To A Set of Independent (Uncoupled) SDOF ODEs and Solving the Independent Equations in a Manner Similar to Solving a SDOF ODE In reality, all systems have distributed mass, damping and stiffness properties. The finite element method discretizes the continuous system with a finite number of degrees of freedom resulting in a set of ordinary differential equations (ODEs) when Newton’s equation of motion is applied. Continuous systems on the other hand result in one partial differential equation. Since the integration of the partial differential equation (PDE) is far more complicated, the modelling of a structure as a continuous system is limited to simple structures. The BernoulliEuler beam equation of motion, which is based on simple bending theory assuming that plane sections remain plane results in the equation of motion ∂ 4u ∂ 2u + m = P(x, t ) ∂x 4 ∂t 2 where u is the transverse displacement. Note that the Timoshenko beam equation extends the Bernoulli-Euler beam theory to include shear deformations and rotary inertia and should be used if such effects matter. Solving the corresponding free vibration PDE analytically by the method of separation of variables leads to two ODEs, which yield the following natural circular frequencies and mode shapes EI EI mL4 ω n = a 2 L2 φ( x ) = A sin ax + B cos ax + C sinh ax + D cosh ax The values of a and the integration constants depend on the boundary conditions and is presented in Section 4.1.3.4. The orthogonality property for continuous systems can be shown to be essentially similar to that of the discrete systems. Hence, if for a discrete system the uncoupled equation of motion for the ith mode is Mi& ξ&i ( t ) + (ζ i 2M i ω n i )ξ&i ( t ) + K i ξ i ( t ) = Pi (t) {φi }T [M ]{φi }& ξ&i ( t ) + (ζ i 2{φ i }T [M ]{φ i }ω n i )ξ&i ( t ) + {φ i }T [K ]{φ i }ξ i ( t ) = {φ i }T {P( t )} Likewise, the uncoupled equation of motion for the ith mode of a continuous system (in particular that of a beam) is Mi& ξ&i ( t ) + (ζ i 2M i ω n i )ξ&i ( t ) + K i ξ i ( t ) = Pi (t) M& ξ&( t ) + (ζ 2M ω )ξ& ( t ) + ω 2 M ξ ( t ) = P (t) i i i i ni i ni i i i L   &  mφ 2 ( x )dx &   2 2  2 & i  0  ξ i ( t ) + ζ i 2 0 mφ i ( x )dx ω n i  ξ i ( t ) + ω ni  0 mφ i ( x )dx  ξ i ( t ) = 0 φ i ( x ){P( x , t )}dx where the modal mass, modal damping, modal stiffness and modal force is clearly determined. There will be n uncoupled ODEs for n natural modes. These are now simply SDOF ODEs, which can be solved using Duhamel’s integral. For a particular mode i, for a general loading function Pi(t), from SDOF response analysis, we can establish Di(t) = dynamic amplification factor in the time domain Note that in general, Di(t) is a function of the natural circular frequency ωni2 = Ki/Mi, the time duration of loading td and the general time t. From this, we can establish the modal responses ξi(t) = modal displacement response in the time domain, Di(t)(p0i/ Ki) Note that p0i corresponds to the amplitude of the modal loading function Pi(t). ∫ L ∫ L ∫ L ∫ The final step is to obtain the physical displacements u(x,t) from the summation of the n modal responses as follows. n u ( x , t ) = φ i ( x )ξ i ( t ) ∑ i =1 As a final note, the element stresses (here the bending moments and shear forces) can be obtained from the Bernoulli-Euler beam equations M ( x , t ) = EI ∂ 2u ∂x 2 V ( x , t ) = EI ∂ 3u ∂x 3 456 Structural Engineering Analysis and Design Second Edition 4.8 4.8.1 GL, ML Implicit Direct Transient Response Analysis Nature of the Dynamic Loading Function The solution can be used to ascertain the modal properties of the system by performing a time domain impulse analysis to excite the modes of interest. The duration of the impulse must be sufficiently long to excite the first fundamental mode, which is usually of concern. This would result in a response that includes the first fundamental mode and most likely higher modes as well. The first fundamental mode is readily ascertained from inspection of the response time history curve at any node. Higher natural frequencies can also be ascertained by performing an FFT on the response curve. The solution method can be used to solve dynamic systems subjected to: (a) Deterministic non-periodic short duration impulse (a.k.a. blast) loading functions with subsequent wave propagation (b) Random non-stationary short duration impulse loading functions The force amplitude does not repeat itself regularly but rises from zero to a series of maxima and minima until settling down to a constant value. The starting transient is significant and so the solution is carried out in the time domain. Estimates of the induced stress in a linear elastic body due to an impulsive blast may be made easily in some cases with a simpler static method of analysis. Section 4.7.4 describes this concept further. If the forcing function is a random non-stationary forcing function such that the random forces start from a lowlevel building up to a maximum then dying away, such as in a seismic event, then exact solution methods are not established. Instead, we could either analyze a set of such events using deterministic transient solution methods and then average or envelope the results or alternatively use the crude response spectrum method which envelopes the response spectra of a series of time histories. In this LINEAR TIME DOMAIN solution, the static response must be added to the dynamic response if the dynamic analysis is performed about the initial undeflected (by the static loads) state with only the dynamic loads applied, hence causing the dynamic response to be measured relative to the static equilibrium position. Hence, the total response = the dynamic response + the static response to static loads. Alternatively, in this LINEAR TIME DOMAIN solution, if the dynamic analysis is performed with the deflected static shape as initial input and the static loads maintained throughout the dynamic excitations, the total or absolute response (static and dynamic) is obtained straight away from the dynamic analysis. Hence total response = dynamic response (which already includes the static response to static loads). 4.8.2 Mathematical Formulation of Analysis In general, modal transient response analysis is used when (i) the model is large (ii) many time steps need to be solved for On the other hand, direct frequency response analysis is employed when (i) the model is small (ii) only a few time steps need to be solved for (iii) the response due to high frequency excitation is required, as this requires many modes to be computed in the modal transient response analysis, the computation of the modes being the costly operation in the modal approach (iv) high accuracy is required as the direct approach does not involve mode truncation 457 Structural Engineering Analysis and Design Second Edition The coupled system of ODEs of the damped vibration equation of motion are given by [M]{& u&( t )} + [C]{u&( t )} + [K ]{u ( t )} = {P( t )} The fundamental structural response is solved at discrete times, typically at fixed integration time steps ∆t. Using a central finite difference representation for the velocity and acceleration, {u&n } = 1 {u n +1 − u n −1 } 2 ∆t 1 {& u&n } = 2 {u n +1 − 2u n + u n −1 } ∆t and replacing into the dynamic equation of motion averaging the applied force over 3 adjacent time steps 1 [M ]{u n +1 − 2u n + u n −1 } + 1 [C]{u n +1 − u n −1 } + 1 [K ]{u n +1 + u n + u n −1 } = 1 {Pn +1 + Pn + Pn −1 } 2 2∆t 3 3 ∆t Collecting terms and making {u n +1} the subject [A1 ]{u n +1} = [A 2 ] + [A 3 ]{u n } + [A 4 ]{u n −1} [A1 ] =  1 [M ] + 1 [C] + 1 [K ] 2 2 ∆t 3   ∆t [A 2 ] = 1 {Pn +1 + Pn + Pn −1} 3 [A 3 ] =  22 [M ] − 1 [K ] 3   ∆t [A 4 ] = − 1 [M ] + 1 [C] − 1 [K ] 2 2 ∆t 3   ∆t The initial conditions {u 0 } and {u&0 } are used to determine the values of {u -1}, {P0 } and {P-1}, {u -1} = {u 0 } − {u&0 }∆t {P0 } = [K ]{u 0 } + [C]{u&0 } {P-1} = [K ]{u -1} + [C]{u&0 } Direct response analysis involves the solution of coupled simultaneous geometrically linear dynamic equilibrium equations. The direct transient solution involves decomposing [A1] and applying to the right-hand-side of the equation. The solution behaves like a succession of static solutions with each time step performing a forwardbackward substitution (FBS) on a new load vector. If ∆t is constant during the entire analysis, the [A1] matrix needs to be decomposed only once. Each progressive step in the analysis is only an FBS of a new load vector. If ∆t is changed, [A1] needs to be decomposed again, which can be costly in large problems. The following damping models are supported by the solution scheme I. elemental damping i. viscous damping Yes ii. structural damping Specified but converted to viscous II. modal damping i. viscous damping No ii. structural damping No III. global proportional viscous damping i. mass proportional damping No ii. stiffness proportional damping Specified but converted to viscous iii. Rayleigh damping No 458 Structural Engineering Analysis and Design Second Edition Elemental viscous damping makes contributions to the [C] matrix. [M ]{& u&( t )} + [C]{u&( t )} + [K ]{u ( t )} = {P( t )} Elemental structural damping will modify the damping matrix as follows  [M ]{& u&( t )} + [C ] +  {u&( t )} + [K ]{u ( t )} = {P ( t )}   where the parameter ω4 converts the structural damping into equivalent viscous damping as the transient response analysis does not permit the use of complex coefficients. 1 ω4 ∑G E [ K E ] Stiffness proportional global viscous damping modifies the dynamic equilibrium equations as follows   G [M ]{& u&( t )} + [C ] + [ K ]{u&( t )} + [K ]{u ( t )} = {P ( t )} ω3   where the parameter ω3 converts the structural damping into equivalent viscous damping as the transient response analysis does not permit the use of complex coefficients. 459 Structural Engineering Analysis and Design Second Edition 4.8.3 MSC.NASTRAN Decks 4.8.3.1 GL, ML Direct Forced Transient Response Analysis $ EXECUTIVE CONTROL SECTION SOL 109 $ CASE CONTROL SECTION $ Sets defining grid ids or element ids SET < Number > = 1 THRU 100, 211, 343, < etc > $ Grid output of displacement, velocity and acceleration with time $ SORT1 lists the results by time whilst SORT2 lists the results by grid id DISPLACEMENT(,) = ALL/ VELOCITY(,) = ALL/ ACCELERATION(,) = ALL/ $ Grid output of applied load vector OLOAD(,) = ALL/ $ Grid output of d-set displacement, velocity and acceleration SDISPLACEMENT(,) = ALL/ SVELOCITY(,) = ALL/ SACCELERATION(,) = ALL/ $ Grid output of SPC forces SPCFORCES(,) = ALL/ $ Element output of force, stress and strain ELFORCE(,) = ALL/ ELSTRESS(,) = ALL/ STRAIN(,) = ALL/ $ Analysis Cards SPC = < ID of SPC Cards Defined in Bulk Data > TSTEP = < ID IN TSTEP > $ XY plot output OUTPUT(XYPLOT) XYPUNCH RESPONSE /() XYPUNCH RESPONSE /() $ BULK DATA TSTEP ID Number of Steps, N1 Time Step, ∆t1 Output Every NO1 Steps Number of Steps, N2 Time Step, ∆t2 Output Every NO2 Steps … etc … The integration time step must be small enough to represent accurately both the variation in the loading and also to represent the maximum frequency of interest. If a loading has a frequency content of 500 Hz then the time step should be less than 1/500 s. A very high frequency transient excitation will have very sharp spikes (i.e. very low period). It is necessary for the integration time step to subdivide this. Another reason is the fact that the solution algorithm smoothes the force by taking the average of 3 times steps. Hence, it is important to avoid defining discontinuous forcing functions. If the analysis calls for sharp impulses, it is best to smooth the impulse over at least one integration time step. It is also recommended to use at least 10 solution time steps per period of response for the cut-off maximum frequency of interest. Hence if the highest frequency of interest is 500 Hz, then the time step should be 1/(500x10) or smaller. Since the solution algorithm is an implicit time integration scheme, the size 460 Structural Engineering Analysis and Design Second Edition of the time step is limited for accuracy purposes and not for the stability of the scheme, which becomes the governing criteria in explicit time integration schemes. It is recommended that the time step not be changed in a linear direct transient analysis. This is because a decomposition of the dynamic matrix is required each time ∆t is changed and this can be a costly operation. Also, a constant ∆t is recommended because an artificial spike occurs each time ∆T is changed, especially if NOLINi is present. As for the duration of analysis, it is important that it be long enough such that the lowest flexible mode oscillates at least through one cycle. So if the first fundamental natural frequency is 0.5 Hz, the duration of analysis should be at the least 2.0 s. In both direct and modal transient response analysis, the cost of integration is directly proportional to the number of time steps. If on one hand, a small time step is required to subdivide the smallest period, a long enough duration of analysis is required to properly capture long period response. This is so because in many cases, the peak dynamic response does not occur at the peak value of load nor necessarily during the duration of the loading. A good rule is to always solve for at least one cycle of response for the longest period mode after peak excitation. To specify the optional initial displacement and velocity conditions (note that initial accelerations is assumed to be zero), $ CASE CONTROL SECTION IC = < ID OF TIC > $ BULK DATA TIC SID Grid ID Component Number Initial Displacement Initial Velocity In this LINEAR TIME DOMAIN solution, the static response must be added to the dynamic response if the dynamic analysis is performed about the initial undeflected (by the static loads) state with only the dynamic loads applied, hence causing the dynamic response to be measured relative to the static equilibrium position. Hence, the total response = the dynamic response + the static response to static loads. Time domain dynamic excitation functions should always be applied from the amplitude of 0.0 (and realistically de-ramped to 0.0 as well). This is because inherently, the dynamic excitation function has to be extrapolated within the analysis code to be from 0.0. Hence, that initial jolt should better be representative of reality irrespective of whether load excitations or enforced motion is being applied. Alternatively, in this LINEAR TIME DOMAIN solution, if the dynamic analysis is performed with the deflected static shape as initial input and the static loads maintained throughout the dynamic excitations, the total or absolute response (static and dynamic) is obtained straight away from the dynamic analysis. Hence total response = dynamic response (which already includes the static response to static loads). Of course, if the transient dynamic analysis follows a static analysis (by say SOL 101, SOL 106, implicit dynamic relaxation by SOL 129 or explicit dynamic relaxation), then the dynamic excitation function should be ramped up from the static amplitude and not from 0.0 (and realistically de-ramped to the static load as well), so that again there would be no jolt unrepresentative of reality. 461 Structural Engineering Analysis and Design Second Edition 4.8.3.1.1 Applied Load Excitations To define a time dependent dynamic excitation, both spatial distribution and the time variation (i.e. the temporal distribution) must be defined. TLOAD1: {P( t )} = {AF(t − τ)} TLOAD2: {P(t )} =  0 , ~ B C~t ~  A t e cos(2πF t + P) , ~ where t = t − T1 − τ t < (T1 + τ) or t > (T 2 + τ) (T1 + τ) ≤ t ≤ (T 2 + τ) t = time A = amplitude scalar multiplier defined by DAREA for a DOF τ = time delay in an applied load defined by DELAY for a DOF F(t) = time dependent force variation defined by TABLED1 T1 = time constant defined by T1 in TLOAD2 T2 = time constant defined by T2 in TLOAD2 F = frequency (cycles per unit time) defined by F in TLOAD2 P = phase angle (degrees) defined by P in TLOAD2 C = exponential coefficient defined by C in TLOAD2 B = growth coefficient defined by B in TLOAD2 $ CASE CONTROL SECTION DLOAD = < ID OF TLOAD1 or TLOAD2 > $ BULK DATA TLOAD1 ID DAREA ID DELAY ID TYPE F(t) TABLED1 ID TLOAD2 ID DAREA ID DELAY ID TYPE T1 T2 F C B DAREA ID GRID ID Component Number Scale Factor GRID ID Component Number Scale Factor DELAY ID GRID ID Component Number Time Delay τ GRID ID Component Number Time Delay τ TABLED1 ID XAXIS YAXIS x1 y1 x2 y2 x3 y3 x4 x5 y5 x6 y6 … … ENDT 462 P Y4 Structural Engineering Analysis and Design Second Edition TYPE is the TLOAD1 and TLOAD2 entries defined the type of excitation, i.e. 0 for Force or Moment. Any number of DAREA and DELAY entries may be defined. All those with the same ID will be subjected to the same dynamic excitation defined in the TLOAD1 and TLOAD2 entries. The XAXIS and YAXIS in the TABLED1 entry refers to either LINEAR or LOG interpolation between and beyond the extremities of the specified {xi , yi} pairs of {time, amplitude}. Hence to define a force that ramps up and is constant thereafter as shown P(t) 4.0 t 2.5 5.0 we define for TLOAD1 A = 4.0 in DAREA τ = 2.5 in DELAY F(t) in a TABLED1 entry F(t) 1.0 t 2.5 Hence, using a TABLED1 we can define very general transient force excitations. To define a sinusoidal harmonic load P(t) = −6.0sin(ω(t−6.7)) with a period T = 0.5s for one cycle (i.e. from t = 6.7s to t = 7.2s), F(t) 6.0 6.7 7.2 T = 0.5s hence, f = 2.0 Hz we define for TLOAD2, A = 6.0 in DAREA τ = 6.7 in DELAY T1 = 0.0 T2 = 0.5 F = 2.0 P = 90.0 degrees C = 0.0 in TLOAD2 B = 0.0 in TLOAD2 463 t Structural Engineering Analysis and Design Second Edition Hence, {P(t )} =  0 , ~ B C~t ~  A t e cos(2πF t + P) , ~ where t = t − T1 − τ {P(t )} =  0 t < 6.7 or t > 7.2 , 6.0 cos(2π2( t − 6.7) + 90.0) Since, sin θ = cos (90.0−θ) {P(t )} =  t < (T1 + τ) or t > (T 2 + τ) (T1 + τ) ≤ t ≤ (T 2 + τ) 0 t < 6.7 or t > 7.2 ,  − 6.0 sin( 2π2( t − 6.7)) 6.7 ≤ t ≤ 7.2 , , 6.7 ≤ t ≤ 7.2 In order to verify the applied loading, the response to the load applied suddenly (over one or two time steps) should be checked to double the results from a static analysis with the same loading. Defining the spatial distribution using DAREA only enables the specification of dynamic concentrated forces and moments. To accommodate more complicated loadings, the LSEQ entry is used to refer to static load entries that define the spatial distribution of the dynamic loads. $ CASE CONTROL SECTION LOADSET = < ID OF LSEQ > DLOAD = < ID OF TLOAD1/TLOAD2 > $ BULK DATA DAREA Reference Link DAREA Reference Link LSEQ ID TLOAD1 ID TLOAD2 ID DAREA Reference Link C B Static Load ID Temp Load ID DELAY ID TYPE F(t) TABLED1 ID DELAY ID TYPE T1 T2 F P The DAREA Reference Link links the TLOAD1/TLOAD2 entry to the LSEQ which can now be used to refer to static load set ids which define the spatial distribution of the dynamic loads. The static load set id can refer to one or more static load entry types. Obviously, there is not a DAREA entry anymore. It is replaced by an LSEQ bulk data entry, a LOADSET case control entry and the pertinent bulk data static load entries such as FORCE, PLOADi or GRAV. The time dependent load card TLOAD1/TLOAD2 is selected using the DLOAD case control command. A new automatic feature will be activated if and only if the user does not have a LOADSET/LSEQ selection. With the new enhancement, it is no longer necessary for the user to explicitly specify LOADSET/LSEQ combination in order to employ static loading data in dynamic analysis. Instead, when the user selects a dynamic load, all static loads and thermal loads that have the same ID as the DAREA ID on the dynamic load entry are automatically selected. If more than one TLOAD1/TLOAD2 entry is required, then a dynamic load set combination is required. This is done using a DLOAD bulk data entry that linearly combines multiple TLOAD1/TLOAD2 entries. 464 Structural Engineering Analysis and Design Second Edition $ CASE CONTROL SECTION DLOAD = < ID OF DLOAD > $ BULK DATA DLOAD 4.8.3.1.2 ID Overall Scale Factor Scale Factor TLOAD1 / TLOAD2 ID Scale Factor TLOAD1 / TLOAD2 ID Nonlinear Transient Load Nonlinear transient loads are as described in nonlinear forced transient response analysis. 465 ..etc.. Structural Engineering Analysis and Design Second Edition 4.8.3.1.3 Enforced Motion Four methods can be used for enforced motion, namely: (i) The direct absolute response approach (ii) The direct relative response approach (iii) The indirect large mass method (absolute response approach) (iv) The indirect large spring method (absolute response approach) The direct absolute response approach makes no assumptions. The direct relative response approach makes the following assumptions 6: (i) (ii) (ii) base movements in any given direction are identical i.e. that the base supports cannot move independently no mass or damping coupling between the structure and the ground (the off diagonal terms in the unsupported mass matrix that couple the structure and the ground movements are zero or are insignificant) no damping into the ground In both the direct absolute and direct relative approaches, the equation of motion is the same on the LHS, hence the same resonant frequencies and mode shapes are obtained, only the applied loading vector on the RHS differ. The two approaches will also give the same stresses within the elements. With the assumption of no coupling of mass and damping, the absolute response is found by applying a base displacement and the relative response by applying a base displacement. The absolute displacement response and relative displacement response only differ by a rigid body movement. 4.8.3.1.3.1 Direct Enforced Motion (Absolute Response Approach) The direct approach of applying enforced motion is the most accurate method. Denoting the free DOFs as f and the constrained DOFs (whether with enforced motion or zero constraints) as s, P the force and q the reaction, the dynamic equilibrium equation can be partitioned as With zero constraints, i.e. the dynamic equation of motion reduces to the usual with the corresponding reactions But, with enforced motion, the dynamic equation of motion is with the corresponding reactions 6 NAFEMS. A Finite Element Primer. NAFEMS Ltd., Great Britain, 1992. 466 Structural Engineering Analysis and Design Second Edition Hence, in general the user specifies the either the support displacement, velocity or acceleration (as all three motions are related to each other in the sense that the velocity is the first derivative and the acceleration is the second derivative of the displacement) and the equation of motion is solved as usual. But for most structural problems, the damping component Bsf (not Bss in the reaction expression) can be ignored and for lumped mass formulations (or at least no coupling to the support freedoms), Msf is zero, hence reducing the equivalent forcing function to Pf(t) – Kfs us(t) and hence, only the base displacement excitation need to be incorporated. However, these approximations need not necessarily be employed in which case the absolute approach has no inherent assumptions. Note that the response will be obtained in absolute terms. This solution method is general and is valid even if different supports are moving with different independent excitations. 4.8.3.1.3.2 Direct Enforced Motion (Relative Response Approach) The dynamic equation of motion in absolute terms with enforced motion has been shown to be M ff & u&f + Bff u&f + K ff u f = Pf ( t ) − (M sf & u&s + Bsf u&s + K fs u s ) Assuming that the base movements in any given direction are identical i.e. that the base supports cannot move independently (arising in only seismic problems, not any other), the structural movements can be expressed relative to the base as u rel = u f − u s Thus M ff & u&rel + B ff u&rel + K ff u rel = Pf ( t ) − (M sf & u&s + B sf u&s + K fs u s ) − (M ff & u&s B ff u&s + K ff u s ) Using the fact that Kus = 0 and assuming further that the mass and damping are diagonal (or at least no coupling to the support freedoms), the equation of motion becomes M ff & u&rel + B ff u&rel + K ff u rel = Pf ( t ) − (M ff & u&s + B ff u&s ) Assuming further that there is no damping into the ground, we obtain the common form M ff & u&rel + B ff u&rel + K ff u rel = Pf ( t ) − M ff & u&s The DLOAD Case Control Command, optionally the DLOAD bulk data entry, TLOAD1/TLOAD2, DELAY and TABLED1 is used in the same way as they were when load excitations were applied. One difference is the TYPE field of TLOAD1/TLOAD2 where instead of load excitation LOAD, enforced motion in terms of DISP, VELO or ACCE is specified. Another difference for the direct enforced motion lies in the EXCITEID Field 3 of TLOAD1/TLOAD2, where instead of referencing a DAREA card (hence not requiring a DAREA card at all for enforced motion), the EXCITEID Field references an SPCD entry, which in turn will reference a GRID ID and an associated DOF component in which the enforced motion is to be applied. Now at the same time, in line with methods of applying enforced motion in static analysis, the DOF component of the GRID ID with enforced motion must be constrained with an SPC bulk data entry which of course must be referenced by an SPC Case Control Command. Modal augmentation vectors by PARAM, RESVEC, YES must be used for modal methods. This is because since there no rigid body modes (as they are constrained by the enforced motion), there can be no motion of the enforced points unless RESVEC is used. 467 Structural Engineering Analysis and Design Second Edition 4.8.3.1.3.3 Indirect Large Mass Method (Absolute Response Approach) – Base Acceleration Specified If a very large mass m0, which is several orders of magnitude larger than the mass of the entire structure, is connected to a DOF where a dynamic load is applied, then the acceleration of the DOF is approximately P( t ) & u&( t ) = m0 Hence, the (large) force required to produce the desired acceleration at the DOF is P(t) = m 0 & u&( t ) The stiffness, damping and the inertial force of the mass of the structure at the DOF contributes little in comparison to the force provided by the large mass, hence the acceleration response is due primarily to the inertial force of the large mass. The larger the mass in comparison, the more accurate the acceleration excitation. However the magnitude is limited by numeric overflow in the computer. MSC recommends that the value of m0 be approximately 106 times the mass of the entire structure for an enforced translational DOF and 106 times the mass moment of inertia of the entire structure for a rotational DOF (for 6 digits of numerical accuracy). The disadvantage of the large mass method is that it involves a loss of numerical conditioning and hence a loss of accuracy of the response. If the large mass is 106 times the mass of the structure, this is equivalent to losing 6 significant figures in the definition of the mass and stiffness matrices. The following procedure is employed to specify prescribed motion in forced transient response analysis: (i) remove constraints from the enforced DOFs (ii) place large masses or inertia scalar elements CMASSi or CONMi with values approximately 106 times the mass or mass moment of inertia of the entire structure (iii) indicate in Field 5 of TLOAD1 or TLOAD2 whether the enforced motion is a displacement, velocity of acceleration; NASTRAN automatically differentiates a specified velocity once or a specified displacement twice to obtain an acceleration; Hence, to maintain accuracy, it is best to specify an acceleration in the first place (iv) apply a dynamic load to each enforced DOF equal to P(t ) = m 0& u&( t ) if accelerati on prescribed motion P ( t ) = m 0 u&( t ) if velocity prescribed motion P ( t ) = m 0 u ( t ) if displaceme nt prescribed motion The DLOAD Case Control Command, optionally the DLOAD bulk data entry, TLOAD1/TLOAD2, DAREA, DELAY and TABLED1 is used in the same way as they were when load excitations were applied. The key difference is the TYPE field of TLOAD1/TLOAD2 where instead of load excitation LOAD, enforced motion in terms of DISP, VELO or ACCE is specified. To ensure that the chosen mass values are high enough two modal analyses (SOL 103) should be run, one with the enforced DOFs constrained and the other with the large masses attached and the DOFs left unconstrained. The flexible frequencies (not the rigid mode frequencies) between the two analyses should be well comparable (to within 4 or 5 significant figures), otherwise the mass values should be increased. In modal methods, further considerations must be made to the rigid body modes. Globally unconstrained structures will have rigid body modes. Releasing a global DOF and placing a large mass there to enforce an applied motion will result in that DOF being unconstrained and hence will result in a rigid body mode (stress free mode). This mode can safely be discarded in the solution by using LFREQ or simply not calculating it in EIGRL. If however two large masses are placed at two different locations to simulate enforced motion in the same direction, there will be a further low-frequency mode that represents the motion of one large mass relative to the other. This mode does contribute to the stresses are cannot be ignored. It must be captured within EIGRL and LFREQ. To avoid this problem, a solution will be to place only one large mass at an arbitrary location and connect with RBE2 elements all DOFs that are to be subjected to that enforced motion. 468 Structural Engineering Analysis and Design Second Edition 4.8.3.1.3.4 Indirect Large Spring Method (Absolute Response Approach) – Base Displacement Specified A stiff spring may be used to simulate an enforced displacement. P(t) = k0 u(t) where k0 is the stiffness of the stiff spring and u(t) is the enforced displacement. The large stiffness method certainly works, but the large mass method is preferred because it is easier to estimate a good value for the large mass than to estimate a good value for the stiff spring. In addition and more importantly, the large mass method is far superior when modal methods are used. If very stiff springs are used for modal analysis rather than very large masses, the vibration modes corresponding to the very stiff springs have very high frequencies and in all likelihood, are not included among the modes used in the response analysis. This is the main reason that large masses should be used instead of stiff springs. The stiff spring method is however advantageous in the case of (time domain) enforced displacement because it avoids the roundoff error that occurs while differentiating the displacement to obtain acceleration in the large mass method. The stiff spring method also avoids the problem of rigid-body drift when applying enforced motion on statically determinate support points (Rigid-body drift means that the displacement increases continuously with time, which is often caused by the accumulation of small numerical errors when integrating the equations of motion). 4.8.3.1.4 Damping To specify stiffness proportional global viscous damping on all the deformable elements, the following parameters are used. $ BULK DATA PARAM,G, PARAM,W3, To specify elemental structural damping on selected deformable elements, PARAM, W4 is used in conjunction with the GE field on the MATi or entries in the CBUSH or CELAS elements to convert the structural damping into equivalent viscous damping. $ BULK DATA PARAM,W4, If PARAM, W3 and/or PARAM, W4 is not specified, it defaults to 0.0, hence ignoring all the elemental structural damping cards. Because time domain solutions cannot handle structural damping, an equivalent viscous damping is required. Hence, if structural damping is specified at the element levels, then the incorrect modal damping will result because the conversion from structural to viscous damping will only be valid for one modal natural frequency, w4 as specified by PARAM, W4 (Note that element viscous damping damps different modes accurately). Hence, if the model has any structural damping, then it should be specified as modal damping. Modal damping can be calculated using SOL 107 and specified as either modal structural or modal viscous damping (hence a modal method of analysis i.e. SOL 112 must be used). Of course, the modal damping will be converted to modal viscous damping for solution in the time domain. This conversion is only perfectly accurate when the frequency of excitation matches the natural frequency of the mode (at resonance), but of course this is acceptable as only that is the instance when the damping estimate is most critical. Note that in the frequency domain, for the modal solution (SOL 111), the modal damping specified will be converted to either modal viscous or modal structural damping depending on PARAM, KDAMP. 469 Structural Engineering Analysis and Design Second Edition 4.8.3.2 GL, ML P-∆ (KGA From KEA) Direct Forced Transient Response Analysis It is often necessary to incorporate the reduction in bending stiffness of gravity load resisting columns for the analysis of lateral loads. The following procedure is undertaken. Phase 1 Perform static analysis (with loads that cause the greatest negative or positive geometric stiffness) based on [KEA] but include the segyroa.v2001 alter prior to the Case Control Section in order to compute the geometric stiffness matrix [KGA]1 (and output into a .pch file) based on the generated element loads from the [KEA] static analysis. Phase 2 A SOL 109 with a general loading function is undertaken based on [KEA] + [KGA]1 with the k2gg=ktjj statement in the Case Control Section and the outputted .pch file which contains the ktjj matrix in the Bulk Data. The responses at this stage represent the P-∆ (KGA From KEA) response to the dynamic excitation. The following equivalent alternative procedure can also be employed. $ CASE CONTROL SECTION SUBCASE 1 LABEL = Static Preload Load Case LOAD = < ID of FORCEi, MOMENTi, PLOADi, GRAV, LOAD, SPCD Cards in Bulk Data > TEMP(LOAD) = < ID of TEMP, TEMPRB, TEMPP1 Cards in Bulk Data > DEFORM = < ID of DEFORM Cards in Bulk Data > SUBCASE 2 LABEL = P-∆ Direct Transient Response Analysis STATSUB(PRELOAD) = 1 DLOAD = < ID OF TLOAD1 or TLOAD2 > The method is valid when only the prestress is judged to affect the geometric stiffness such as in the compressive preload of building columns due to gravitational loads and the prestressing of extremely taut cables that sag very little under gravity but not in systems such as suspension bridges. Where lateral loads are large enough to affect the geometry of the system with prestress, then a repetitive P-∆, SOL 106, implicit dynamic relaxation SOL 129 or explicit dynamic relaxation must be employed. But in single P-∆ analysis, because cables do not have much elastic bending stiffness, the initial static preload subcase should only include the prestress and not gravity as including gravity is the same as solving two linear static problems of stiffness KEA with preload and gravity as the applied loads respectively. Clearly, in the gravity case, it is nonsensical as the cables do in reality have differential stiffness (from the prestress) to resist the gravitational force. Prestress in one direction (i.e. along the axis of cable) will cause a differential stiffness in the orthogonal direction. Gravity acts in the orthogonal direction and hence cannot be accounted for in the calculation of the prestress in this single P-∆ analysis. To quantitatively decide if gravity need not be considered in contributing to the differential stiffness of the cables, a static P-∆ analysis should be carried out, the first subcase being a SOL 101 with only the prestress as applied loads and the second subcase a P-∆ SOL 101 (i.e. utilizing the induced prestress from the first subcase to form a geometric stiffness matrix) with both the gravity and prestress included as applied loads. If the difference in the cable element forces between subcases 1 and 2 is negligible, then gravity has little influence in affecting the geometric stiffness. If there is a major difference in the cable element force, then clearly, gravity will affect the geometric stiffness and as such, a repetitive P-∆ , SOL 106, implicit dynamic relaxation or explicit dynamic relaxation must be used to converge to the true KT. Likewise, in the single P-∆ analysis of multi-storey buildings, gravity (and only gravity) acts in axis of columns to generate prestress, and the differential stiffness is computed for the orthogonal direction reducing resistance to lateral wind forces, applied in the second subcase with gravity too. 470 Structural Engineering Analysis and Design Second Edition When a static subcase is specified for linear transient response analysis (SOLs 109 and 112) with STATSUB(PRELOAD), the data recovery is controlled by PARAM, ADSTAT. By default (YES) the static solution will be superimposed on the dynamic response solution (displacement, stress and SPCForce). The relative solution can be obtained in reference to the static solution point by PARAM, ADSTAT, NO. No provision is made for frequency response analysis, because the static responses contribute only to the zero frequency response. For linear dynamic response, the static solution can be superimposed after the dynamic solution procedure. The preload effect is reflected only in the stiffness and the actual static load is omitted in the dynamic response analysis. The total displacement can be obtained by superposing the static solution to the transient response analysis. And the stress output is obtained as The STATSUB(PRELOAD) computes the differential stiffness due to the prestress and also the follower force. The follower force is calculated and incorporated by the use of PARAM, FOLLOWK, YES. We know how the prestress affects the differential stiffness, namely a tensile prestress causing an increase in stiffness. The effect of the follower force on the stiffness is different. For example, for a cylinder under external pressure critical buckling load may be overestimated (even though the mode shapes are similar) in a SOL 105 and the natural frequencies in vibration may be underestimated (even though the mode shapes are similar) in a SOL 103 in the absence of follower stiffness. To the contrary, this observations are reversed in case of centrifugal loads. Centrifugal forces as a constant (static) load are applied by a Bulk Data RFORCE to any elements that have masses. The follower stiffness due to centrifugal load has the effect of lowering stiffness (although the centrifugal load tensioning effect increases stiffness), consequently lowering natural frequencies (even though the mode shapes are similar) in a SOL 103 and lowering the buckling loads (even though the mode shapes are similar) in a SOL 105. This effect increases as the RPM increases, and it becomes significant when the RPM is over 1000. For moderately geometric nonlinear analysis, exclusion of follower stiffness affects the rate of convergence, but the converged solution is correct. For severely geometric nonlinear analysis, it may not be possible to obtain a converged solution without including follower stiffness. As the geometric nonlinearity intensifies, so is the effect of follower stiffness. Therefore, inclusion of follower stiffness greatly enhances the convergence if the deformation involves severe geometric nonlinearity. 471 Structural Engineering Analysis and Design Second Edition 4.8.3.3 GL, ML P-∆ (KGA From Exact or Approximate KTA) Direct Forced Transient Response Analysis It is often necessary to include the differential stiffness, especially if there are prestressed cables in the model. To obtain KTA, to be theoretically exact, a GNL SOL 106 (or implicit dynamic relaxation SOL 129 or explicit dynamic relaxation LS-DYNA) with prestress (as temperature loads say) and gravity must be undertaken. Alternatively, an approximation to KTA can be obtained by repetitive P-∆ static analyses with the prestress (as temperature loads say) and gravity applied. The procedure to obtain this approximate KTA will be presented. Note that the approximate KTA will be the summation of the elastic stiffness KE at the undeflected (by the prestress and gravity) state but KG at the deflected (by the prestress and gravity) state. Hence if KE changes considerably during the application of the prestress, a full SOL 106 (or implicit dynamic relaxation SOL 129 or explicit dynamic relaxation LS-DYNA), which converges to the KE and KG at the deflected (by the prestress and gravity) state should be employed. Hence for the modelling of a suspension bridge where there is a great change in geometry (known in the bridge industry as form-finding, so-called because it is necessary to find the form or shape of the catenary suspension cables), it may be prudent to employ SOL 106 (or implicit dynamic relaxation SOL 129 or explicit dynamic relaxation LSDYNA), but for a high tension low sag cable on say a tower with prestressed cables, the repetitive P-∆ static analysis may be adequate. The repetitive P-∆ analysis basically involves a number of iterations of linear static analyses to obtain an approximate KTA. Note again that A refers to the initial undeflected (by the collapsing load) state, but deflected by the prestress and gravity. To perform the repetitive P-∆ analysis, a static analysis is performed based on KEA with temperature loads and gravity to generate forces in the structural elements, which in turn provides input for the computation of KGiAKTm where m is the iterations. Repetitive static analysis is performed with the prestress and gravity updating the stiffness matrix KEA + KGiAKTm-1 + KGiAKTm until convergence of displacements is obtained. The tangent stiffness at this stage is the approximate converged tangent stiffness matrix KTA = KEA + KGiAKT. The converged displacements represent the approximate P-∆ (KGA From Approximate KTA) static response to the initial prestress loads. The converged geometric stiffness at this stage would be that based upon the approximate tangent stiffness matrix KTA, i.e. KGiAKT. Phase 1 Perform static analysis (with prestress and gravity) based on [KEA] but include the segyroa.v2001 alter prior to the Case Control Section in order to compute the geometric stiffness matrix [KGA]1 (and output into a .pch file) based on the generated element loads from the [KEA] static analysis. Phase 2 Perform static analysis (with prestress and gravity) based on [KEA] + [KGA]1 by including the k2gg = ktjj statement in the Case Control Section, the outputted .pch file which contains the ktjj matrix in the Bulk Data and the segyroa.v2001 alter prior to the Case Control Section to compute the [KGA]2 (and output into the .pch file overwriting previous data) based on the generated element loads from the [KEA] + [KGA]1 static analysis. Phase 3 Repeatedly perform the Phase 2 static analysis (with prestress and gravity) based on [KEA] + [KGA]i for i = 2 to n where n represents the number of iterations required for the change in deflections between analyses to become negligible. This would signify that the change in the [KGA] matrix become negligible and the correct [KGA] is attained. The deflections and the other responses at this stage represent the P-∆ (KGA From Approximate KTA) static response to the prestress and gravity. The stiffness of the structure is KTA. Phase 4 A SOL 109 with a general loading function is undertaken with the k2gg=ktjj statement in the Case Control Section and the outputted .pch file which contains the latest ktjj matrix in the Bulk Data. The responses at this stage represent the P-∆ (KGA From Approximate KTA) response to the dynamic excitation. 472 Structural Engineering Analysis and Design Second Edition 4.8.4 Hand Methods Verification 4.8.4.1 Determination of Maximum Dynamic Displacement, umax by Solving the SDOF Undamped/Damped Linear Equation of Motion ODE for Deterministic Time Domain Loading With/Without Initial Conditions Using the Convolution Integral (Duhamel’s integral) The Duhamel’s integral can be used to calculate the response of SDOF systems to general loading functions. It inherently includes both the steady state and the transient components of the motion in the response corresponding to no initial conditions. However, the method is only valid for linear elastic structures as superposition of response is utilized. The impulse of a force is defined as the product of the force p(τ) and its duration time dτ. An impulsive force acts only for a short duration of time. We define time a general time variable τ where τ = 0 Initial displacement and velocity conditions τ = τ Time of application of impulsive force for duration dτ τ = t Time dynamic response sought p(τ) dτ τ t From Newton’s Laws of Motion, an impulse on a mass m will result in a change of momentum and hence change of velocity. mdv = p(τ)dτ τ τ+dτ p(τ)dτ m This incremental velocity can be considered as the initial velocity of a free vibrational analysis. Recall the transient state solution for a free vibrational analysis with initial displacement and velocity conditions. u&(0) u(t) = sin ω n t + u (0) cos ω n t ωn dv = Hence the response due to the initial velocity dv (with no initial displacement) at time τ at a later time t, du (τ = t ) = p ( τ) dτ sin ω n (t − τ ) mω n We denote the start of the application of the impulsive forces at time τ (for duration dτ) and the response to be evaluated at time t. A general loading function can be regarded as a series of short impulses at successive incremental times of dτ, each impulse producing its own differential response at time t. Thus, the total response at t will be the superposition of all the impulses acting from time τ = 0 to τ = t. ∫ τ= t τ=0 du ( τ = t )dτ = u (τ = t ) = 1 mω n ∫ ∫ τ= t τ=0 τ= t τ=0 p ( τ ) dτ sin ω n (t − τ ) mω n p(τ) sin ω n (t − τ )dτ This is known as the Duhamel’s integral and it inherently includes both the transient state and steady state components of the response. Because it utilizes superposition of the responses, it is only valid for linear elastic structural behavior. To also incorporate initial conditions at time τ = 0, u (τ = t ) = u&( τ = 0) 1 sin ω n t + u ( τ = 0) cos ω n t + ωn mω n ∫ τ= t τ=0 473 p( τ) sin ω n (t − τ )dτ Structural Engineering Analysis and Design Second Edition Including viscous damping, the corresponding expression becomes   u&( τ = 0) + u ( τ = 0)ζω n 1 u ( τ = t ) = e −ζωn t  u ( τ = 0) cos ωd t + sin ωd t  + ωd   mωd ∫ τ= t τ=0 p(τ)e −ζωn ( t − τ ) sin ωd (t − τ )dτ where ωd = ω n 1 − ζ 2 Hence, the general Duhamel’s Integral expression excluding the initial conditions, u (τ = t ) = where h(t - τ) = and h(t - τ) = ∫ τ= t τ=0 p(τ)h ( t − τ)dτ 1 sin ω n ( t − τ) without damping mω n 1 e − ξωn ( t − τ) sin ω d ( t − τ) with damping mω d Incidentally, h(t-τ) is known as the unit impulse response function. Now it is just a matter of evaluating this integral and expression either classically or numerically for a variety of loading functions to determine the response. Other quantities such as velocity and acceleration can be obtained simply by differentiating the displacement expression with respect to t. Sometimes this simply results in a multiplication by ωn (or ωd) for velocity and ωn2 (or ωd2) for acceleration. (i) An Instantaneous Impulsive Force of Duration t1 < T An impulse is a very large load acting for a very short time. So long as t1/T < 0.2, we can approximate the force as an impulse. The lower the t1/T, the more impulse-like the loading becomes. An impulse analysis is easier because h(t-τ) can be approximated outside the integral whereas in the non-impulse loading h(t-τ) must be evaluated inside the integral. The remainder within the integral reduces to simply the area (or impulse) under the loading force p(τ). u ( τ = t ) = h(t - τ) ∫ τ= t τ= 0 p(τ)dτ u(τ = t) = τ= t 1 sin ω n ( t − τ) ∫ p(τ)dτ undamped τ= 0 mω n u(τ = t) = τ= t 1 e −ξωn ( t − τ ) sin ω d ( t − τ) ∫ p(τ)dτ damped τ =0 mω d τ= t u max = 1 mω n ∫τ=0 p(τ)dτ u max = 1 mω d ∫τ=0 p(τ)dτ τ= t undamped damped Another equivalent interpretation of the above relationship is from the basic consideration of the conservation of momentum. The impacting particle (of small relative mass compared to mass of structure) imposes an impulse I onto the structure. The magnitude of I can be calculated as m∆v where m is the small mass and ∆v the change of velocity at impact. If there is no rebound ∆v is the approach velocity. Conservation of momentum at impact requires the initial velocity of the structural mass to be I/M. A lightly damped system then displays damped free vibration with an initial displacement of approximately I/(ωdM), or an initial velocity of approximately I/M or an initial acceleration of approximately Iωd/M. 474 Structural Engineering Analysis and Design Second Edition (ii) An Instantaneous Continuous Constant Force of Amplitude p0 p(τ) p0 τ τ=t With no damping, u (τ = t ) = ∫ τ= t τ =0 =∫ p ( τ) τ= t τ =0 = = p0 p0 mω 2n 1 sin ω n ( t − τ)dτ mω n 1 sin ω n ( t − τ)dτ mω n cos ω n (t − τ) 0 t p0 (1 − cos ω n t ) k 2p 0 when cos ω n = −1 k The maximum dynamic displacement is twice the static displacement. This means that a constant force applied suddenly will produce a maximum displacement of twice that which will be produced if the force was applied statically (i.e. slowly such that there are no dynamic effects). This is also true for internal forces and stresses. u max = 475 Structural Engineering Analysis and Design Second Edition (iii) An Instantaneous Rectangular Force of Duration td of Amplitude p0 p(τ) τ τ=t τ = td p0 With no damping, For τ < t d p0 (1 − cos ω n t ) k p u&(τ = t ) = 0 ω n sin ω n t k 2p u max = 0 k For τ = t d u (τ = t ) = p0 (1 − cos ω n t d ) k p u&(τ = t d ) = 0 ω n sin (ω n t d ) k For τ > t d , we utilize the initial conditions as at τ = t d , hence replacing t by t − t d u&(τ = t d ) 1 τ= t u (τ = t ) = sin ω n (t − t d ) + u (τ = t d ) cos ω n (t − t d ) + p(τ) sin ω n (t − τ)dτ mω n ∫τ = t d ωn u (τ = t d ) = p0 k p0 u (τ = t ) = k p u (τ = t ) = 0 k u (τ = t ) = sin (ω n t d ) sin ω n (t − t d ) + p0 (1 − cos ω n t d ) cos ω n (t − t d ) + 0 k (cos ω n (t − t d ) − cos ω n t ) − td  2t − t d  sin ω n  − 2 sin ω n  2 2   p t 2t − t d u max = 2 0 sin ω n d when sin ω n =1 k 2 2 It is found that the maximum dynamic response is a function of ωntd or td/T. For td/T ≥ 0.5, the maximum dynamic response is the same as it would have been had the force loading been infinite. This means that the maximum amplification occurs during the application of loading. However, if the loading is very short duration, such that td/T < 0.4, than the maximum response may occur after the loading, during the subsequent free vibration. 476 Structural Engineering Analysis and Design Second Edition (iv) An Instantaneous Right Angled Triangular Force of Amplitude p0 p(τ) τ = td p0 τ With no damping, For τ < t d u (τ = t ) = p0 (1 − cos ωn t ) + p 0 k kt d  sin ω n t   − t   ωn  For τ > t d , u (τ = t ) = p0 (sin ωn t − sin ωn (t − t d )) − p 0 cos ωn t kωn t k As always, a plot of y(t) versus td/T would be very beneficial. For large values for instance in this case, the maximum dynamic displacement response approaches twice the static displacement value. (v) An Instantaneous Isosceles Triangular Force of Amplitude p0 p(τ) τ = td p0 τ With no damping, For τ < t d / 2 u (τ = t ) = 2p 0 (ωn t − sin ωn t ) kω n t d For t d / 2 < τ < t d u (τ = t ) = 2p 0 [ωn (t d − t ) + 2 sin ωn ( t − t d / 2) − sin ωn t ] kω n t d For τ > t d , u (τ = t ) = 2p 0 [2 sin ωn (t − t d / 2) − sin ωn t − sin ωn (t − t d )] kω n t d An impacting particle (of small relative mass compared to mass of structure) imposes an impulse I = F∆t onto the structure. The magnitude of I = F∆t can be calculated as m∆v where m is the small mass and ∆v the change of velocity at impact. If there is no rebound ∆v is the approach velocity. Knowing that F∆t is the area under the impulse curve, making an estimate of the shape of the impulse curve and the duration ∆t, we can thus estimate the peak amplitude. Hence, the impulse curve is defined. 477 Structural Engineering Analysis and Design Second Edition (vi) An Instantaneous Half Sine Force of Frequency ω and Amplitude p0 With no damping, For τ < t d u (τ = t ) = p0 ( k 1− ω 2 / ω 2n )   ω  sin ωt − sin ω n t  ωn   For τ > t d , u (τ = t ) = − ( p 0 ω / ωn k 1 − ω 2 / ω 2n ( ) sin ω t + sin ω n n (t − t d )) An impacting particle (of small relative mass compared to mass of structure) imposes an impulse I = F∆t onto the structure. The magnitude of I = F∆t can be calculated as m∆v where m is the small mass and ∆v the change of velocity at impact. If there is no rebound ∆v is the approach velocity. Knowing that F∆t is the area under the impulse curve, making an estimate of the shape of the impulse curve and the duration ∆t, we can thus estimate the peak amplitude. Hence, the impulse curve is defined. (vii) General Piecewise Linear Loading Functions General piecewise linear functions can be integrated and can be shown to produce response given by the following. Without damping, u (τ = t ) = 1 (A(t ) sin ωn t − B(t ) cos ωn t ) mωn where A( t ) = and B( t ) = ∫ τ= t τ= 0 ∫ τ= t τ= 0 p(τ) cos ω n τdτ = i =n ∑ A(t ) + ∫ i −1 t i −1 i =1 p(τ) sin ω n τdτ = i= n ∑ B(t ) + ∫ i −1 i =1 ti ti t i −1 p(τ) cos ωn τdτ p(τ) sin ω n τdτ where n is the number of linear segments. If the loading is segmented piecewise linearly by ∆t i , the loading function within each segment is p(τ) = p( t i −1 ) + ∆p i (τ − t i−1 ) ∆t i for t i-1 ≤ τ ≤ t i where ∆p i = p( t i ) − p( t i −1 ) and ∆t i = t i − t i −1 On substituti on into the above integrals, and with integration, A ( t i ) = A ( t i −1 ) + +  ∆p  p( t i −1 ) − t i−1 i ∆t i   (sin ωn t i − sin ω n t i−1 )  ∆p i [cos ωn t i − cos ωn t i−1 + ωn (t i sin ωn t i − t i−1 sin ωn t i−1 )] ω 2n ∆t i B( t i ) = B( t i −1 ) + + 1 ωn 1 ωn  ∆p  p( t i −1 ) − t i −1 i ∆t i   (cos ω n t i −1 − cos ωn t i )  ∆p i [sin ωn t i − sin ωn t i−1 − ωn (t i cos ωn t i − t i−1 cos ωn t i−1 )] ω 2n ∆t i The above expressions represent the response at a time during the application of the loading. If the response during the ensuing free vibration is sought, then the expression must be evaluated at the end point of the loading and the initial conditions expression must be used. 478 Structural Engineering Analysis and Design Second Edition (viii) General Nonlinear Loading Functions General loading functions that cannot be classically integrated must be integrated numerically using integration techniques such as Simpson’s Rule. Without damping, u (τ = t ) = 1 mωn ∫ τ= t τ= 0 = sin ω n t p( τ) sin ωn ( t − τ)dτ 1 mωn ∫ τ= t τ= 0 p(τ) cos ω n τdτ − cos ωn t 1 mω n ∫ τ= t τ =0 p(τ) sin ωn τdτ The integrals can be evaluated numerically with Simpson’s Rule which is piecewise parabolic. h (I1 + 4I 2 + 2I 3 + ... + 2I n −2 + 4I n −1 + I n ) 3 In order to use Simpson’s Rule effectively, divide the integral functions into segments, within which the function can be well approximated by a cubic variation. Having three terms I1, 4I2 and I3 is sufficient to model a cubic function exactly. Thus basically, we segment the integral function into piecewise cubic functions and apply Simpson’s Rule separately on each segment, summing the results in the end. Integral = The above expressions represent the response at a time during the application of the loading. If the response during the ensuing free vibration is sought, then the expression must be evaluated at the end point of the loading and the initial conditions expression must be used. 479 Structural Engineering Analysis and Design Second Edition 4.8.4.2 Determination of Maximum Dynamic Displacement, umax by Solving the SDOF Undamped/Damped Linear Equation of Motion ODE (In Relative Terms) for Deterministic Time Domain Support Motion (Displacement, Velocity or Acceleration) With/Without Initial Conditions Using the Convolution Integral (Duhamel’s integral) m& u&( t ) k(u(t)- us(t)) m u(t) c(u&( t ) − u&s ( t ) ) us(t) In absolute terms, the equation of motion m& u&( t ) + c(u&( t ) − u&s ( t ) ) + k (u ( t ) − u s ( t ) ) = 0 In relative terms u r ( t) = u( t) − u s (t ) Hence, m(& u&r ( t ) + & u&s ( t ) ) + cu&r ( t ) + ku r ( t ) = 0 m& u&r ( t ) + cu&r ( t ) + ku r ( t ) = − m& u&s ( t ) Note that in absolute terms, we need the support displacement and velocity in the equation of motion whilst in relative terms we need only the support acceleration in the equation of motion. This resulting equation of motion above is similar to that which considers time domain force loading p(t), and thus can be solved in exactly the same manner taking p(t ) = − m& u&s ( t ) The response will be obtained in relative terms as follows. With damping, u r (τ = t ) = 1 mωd = 1 mωd = 1 ωd ∫ ∫ τ= t τ =0 ∫ τ= t τ =0 τ= t τ= 0 p(τ)e −ξωn ( t − τ) sin ωd ( t − τ)dτ − m& u&s (τ)e −ξωn ( t − τ) sin ωd ( t − τ)dτ −& u&s (τ)e −ξωn ( t −τ ) sin ωd ( t − τ)dτ 1 MAX  ωd  1 = Sv ωd u r max (τ = t ) = ∫ τ= t τ= 0 & u&s (τ)e −ξωn ( t −τ ) sin ωd ( t − τ)dτ  where S v = pseudo spectral velocity 480 Structural Engineering Analysis and Design Second Edition 4.9 4.9.1 GNL, MNL Implicit and Explicit Direct Transient Response Analysis Nature of the Dynamic Loading Function The solution can be used to ascertain the modal properties of the system by performing a time domain impulse analysis to excite the modes of interest. The duration of the impulse must be sufficiently long to excite the first fundamental mode, which is usually of concern. This would result in a response that includes the first fundamental mode and most likely higher modes as well. The first fundamental mode is readily ascertained from inspection of the response time history curve at any node. Higher natural frequencies can also be ascertained by performing an FFT on the response curve. The solution method can be used to solve dynamic systems subjected to: (a) Deterministic non-periodic short duration impulse (a.k.a. blast) loading functions with subsequent wave propagation (b) Random non-stationary short duration impulse loading functions (c) Projectile (a.k.a. impact) excitations with subsequent wave propagation (Explicit Analysis Only) (d) Brittle snap or redundancy check excitations (Explicit Analysis Only) In blast, impact and brittle snap problems, the force amplitude does not repeat itself regularly but rises from zero to a maximum or a series of maxima until settling down to a constant value. The starting transient is significant and so the solution is carried out in the time domain. If the forcing function is a random non-stationary forcing function such that the random forces start from a lowlevel building up to a maximum then dying away, such as in a seismic event, then exact solution methods are not established. Instead, we could either analyze a set of such events using deterministic transient solution methods and then average or envelope the results or alternatively use the crude response spectrum method which envelopes the response spectra of a series of time histories. In this NONLINEAR TIME DOMAIN solution, the static response must be added to the dynamic response if the dynamic analysis is performed about the initial undeflected (by the static loads) state with only the dynamic loads applied, hence causing the dynamic response to be measured relative to the static equilibrium position. Hence, the total response = the dynamic response + the static response to static loads. Alternatively, in this NONLINEAR TIME DOMAIN solution, if the dynamic analysis is performed with the deflected static shape as initial input and the static loads maintained throughout the dynamic excitations, the total or absolute response (static and dynamic) is obtained straight away from the dynamic analysis. Hence total response = dynamic response (which already includes the static response to static loads). 481 Structural Engineering Analysis and Design Second Edition 4.9.2 Deterministic Non-Periodic Short Duration Impulse (a.k.a. Blast) Loading Functions With Subsequent Wave Propagation Estimates of the induced stress in a linear elastic body due to an impulsive blast may be made easily in some cases with a simpler static method of analysis. Section 4.7.4 describes this concept further. Key wavefront parameters are ps peak overpressure Ts positive phase duration is specific impulse (area under pressure-time curve) ta arrival time of blast wave These are well established Rankine-Huginot 1870 W = charge weight R = distance from charge Blast wave scaling laws R1/R2 = (W1/W2)1/3 Scaled distance Z R/W1/3 = Spherical airburst – baseline condition and Hemispherical surface burst – typical condition for terrorist attack. 482 Structural Engineering Analysis and Design Second Edition 4.9.3 Projectile Crash (a.k.a. Impact) (and Impulsive Blast) Analysis With Subsequent Wave Propagation A projectile crash analysis involves the specification of an initial velocity. Hence the a structure is given an initial momentum. The motion is then subsequently retarted when it impacts another elastic body. The impulse (i.e. force) generated depends on the duration taken to retard the momentum, i.e. the impulsive force is the change in momentum divided by the duration. This duration is a function of the stiffness of the elastic body. This is essentially the difference between a projectile crash analysis and a blast analysis, the latter of which has a predefined impulsive force which is independent of the stiffness of the retarding elastic body. Now a consequence of the fact that the force in a projectile analysis being dependent upon the stiffness of the elastic body is that the result of the analysis is very much dependent upon the assumptions made of these stiffnesses. A blast analysis presents a predefined impulsive force and the response of the different modes of the structure is simply dependent upon the predefined magnitude of the impulsive force and the dynamic amplification (which is dependent upon td/Ti where td is the duration of the impulse and Ti the period of the mode, noting that the theoretical maximum dynamic amplification is only 2.0). Now on the other hand, a projectile impact analysis does not predefine the magnitude of the impulsive force. It just defines the momentum. The impulsive force is the change of momentum divided by the duration of the impulse. A stiff retarting structure will offer a short retarding duration and hence resulting in large internal force magnitudes. The impulsive dynamic amplification will still be at most 2.0, but the magnitude of the force could be quite considerable. Hence the definition of the stiffness of the structure retarding the motion is of paramount importance in any projectile impact analysis. Any projectile crash will set off a wave propagation. (Note that an impulsive blast will also set off a wave propagation). As the wave propagates through the structure, parts of the structure that are initially at rest are suddenly forced into motion as the wavefront passes. The highest frequency wave that can be propagated depends upon the distance between consecutive nodes. If the highest frequency to be propagated is f Hz and the wave velocity is v m/s, then the wavelength is λ = v/f. There should be at least 4 nodes over this wavelength for the wave to propagate 7. (Another way of looking at this concept is when stresses resulting from an impulsive blast is to be obtained using modal methods, of course limited to linear analyses; in order for stresses originating from high excitation frequencies to be captured, the mesh has got to be sufficiently fine to represent the higher natural modes as they are the ones that will be amplified the most). A uniform mesh of elements that have all sides of the same length will allow waves to propagate equally in any direction. If a change in mesh density is used within the model, then this gives rise to a change in the effective numerical impedance where the mesh density changes. A fine to coarse mesh transition acts as a filter for the high frequency waves that can be transmitted by the fine mesh but not by the coarse mesh. Hence, spurious high frequency internal wave reflections occur back into the fine mesh at these mesh density changes. Hence a uniform mesh is paramount to wave propagation problems. Wave propagation analysis is performed using an explicit time integration scheme with the time step slightly less than the time is takes the wavefront to travel between two adjacent nodes. If the time step is longer than that, there is an effective truncation of the highest frequency that can be propagated, and if shorter then an excessive amount of computation is carried out unnecessarily. Condensation techniques that truncate high frequency modes of the structure should NOT be used for wave propagations problems. Although high frequency modes of the equations of motion have no physical meaning that are important numerically for wave propagation problems, if they are not included then the wavefront gets dispersed and ceases to be as sharp as they should be. Hence it can be concluded that unlike other dynamic analysis problems, higher modes of vibration is paramount in wave propagation problems (i.e. projectile impact and impulsive blast analysis). Strain-rate effects often are important for projectile crash (and impulsive blast for that matter as that is also a form of wave propagation problem) analysis. The Cowper-Symonds rules are a common simplified method of accounting for strain-rate effects in a MNL solution. Strain-rates will affect the stress-strain curve in a number of ways, namely 7 NAFEMS. A Finite Element Primer. NAFEMS Ltd., Great Britain, 1992. 483 Structural Engineering Analysis and Design Second Edition I. The ‘static’ (i.e. low strain-rate, about 1E-6) stress-strain curve is modified by the Cowper-Symond factor (which is completely defined by the parameters C and P), i.e. a higher strain-rate yields higher stress values. II. The ultimate failure strain is also dependent upon the strain-rate, i.e. a higher strain-rate causes a lower failure strain. The Cowper-Symond values itself are strain dependent. III. For S275 and S355 steel, typical Cowper-Symond C and P parameters are as follows. These result in the following Cowper-Symond factors. However, the strain-rate of the material during testing must also be taken into account. This occurs because the strain-rate at the necking area is greater than elsewhere. (Note that we have already taken the fact that the necking area is smaller in the derivation of the ‘static’ stress-strain curve, this being the engineering stress-strain to the true stress-strain conversion). The following enhancement factors would be applicable for the standard test rates for “static tests”. The absolute strain-rate enhancement, taking the test rate into account, is presented in the table below. For the S275 and S355 carbon steels the failure true strain of 19.9% is derived from the basic tensile test on a standard test coupon. This elongation is measured over the whole test specimen and is therefore not representative of the actual strain in the necked region of the test specimen. The strain in the necking region is based on the reduction in cross-sectional area of the specimen at the necking point. Unfortunately, this is not usually measured during the standard tensile test, but is typically about 50-60% for these carbon steels. 484 Structural Engineering Analysis and Design Second Edition BS 6399-1 specifies accidental vehicle impact loads as follows. 485 Structural Engineering Analysis and Design Second Edition 4.9.4 Brittle Snap or Redundancy Check Excitation A brittle snap or redundancy check analysis include the analysis of sudden fracture of structural members from the static equilibrium configuration such as the sudden snapping of a prestressed structural cable, and evaluates the redundancy available within the structure. This analysis always involves a two-stage procedure. The first stage involves a static solution by a linear static method or a nonlinear static method (either Newton’s tracing the equilibrium path SOL 106, an implicit dynamic relaxation by SOL 129 or an explicit dynamic relaxation method LS-DYNA) in order to obtain the deflected configuration and the stiffness of the structure in the deflected configuration KT by the prestress (prestressing of structural members such as cables contribute greatly to a large change in stiffness within the static solution and hence will require a nonlinear static method) and gravity. The second stage involves a restart into a nonlinear transient dynamic solution scheme with no additional dynamic excitation but with a change in the structure (in the deletion of a member that fails in brittle fashion simulating a redundancy check) or a change in boundary condition (to simulate the effect of the loss of a support or anchor attached to a prestressed cable etc.). An example would be the gradual prestressing of structural cable elements within a suspension bridge or a cable prestressed tower until a static solution (by SOL 106, implicit SOL 129 or explicit LS-DYNA) is achieved. The cables can be prestressed using a gradual temperature load case (or a gradual enforced displacement on the cable anchorage points) plus gravitational loads until the correct level of prestress is achieved (by SOL 106, implicit SOL 129 or explicit LS-DYNA). Then with a restart into an explicit transient dynamic scheme of LS-DYNA, the boundary condition supporting the cable is released or a cable element is deleted, causing the structure to experience an out-of-balance of forces and hence vibrate to a new static equilibrium configuration. The Heathrow T5 Visual Control Tower was analyzed to a sudden brittle cable failure. An initial dynamic relaxation phase was performed (in LS-DYNA) in order to attain the static equilibrium position under gravity load with the correct pretension in the cables. The prestress in the cables was applied by a prescribed displacement at the cable anchorages in the direction along the cable axis during the dynamic relaxation phase until the force in cables reached a value of approximately 1.59MN. At this stage it is a good idea to confirm the natural frequency of the model by applying an impulsive force of say 0.3 seconds (knowing the fundamental mode to be approximately 0.95Hz) duration at the top of the tower. The frequency of the displacement response is observed to be approximately 0.95 Hz. 486 Structural Engineering Analysis and Design Second Edition Static Phase Application of Impulse This correlates well with the natural modes analysis performed in previous linear NASTRAN analyses. 487 Structural Engineering Analysis and Design Second Edition For reference, the natural frequencies of all modes up to 50Hz are presented as follows. The modal masses (normalized to MAX unity) are also presented for this elegant 680.9 tonne structure. T5 VCR REAL MODAL ANALYSIS - FREQUENCY 4.000 Cable Modes 3.500 Secondary Tower Bending Modes Frequency (Hz) 3.000 2.500 Cable Modes 2.000 Primary Tower Torsion Mode Cable Modes 1.500 Cable Modes 1.000 Primary Tower Bending Modes 0.500 0.000 0 5 10 15 20 25 30 35 40 45 50 Mode Number T5 VCR REAL MODAL ANALYSIS - MODAL MASS 250.000 S econdary Tower Bending Modes 225.000 Modal Mass (Tonnes) 200.000 175.000 150.000 Primary Tower Torsion Mode Primary Tower Bending Modes 125.000 100.000 75.000 50.000 Cable Modes Cable Modes Cable Modes Cable Modes 25.000 0.000 0 5 10 15 20 25 30 35 40 45 50 Mode Number The static solution was followed by a transient dynamic phase where the displacement constraint in one of the cables was released, effectively modelling the consequence of a cable suddenly snapping. The resulting effect on the structure is of an impulse of certain duration. On animation of the displacement response (with or without a vector animation of the velocity response), it can be observed if higher modes were excited or not as this will affect the distribution of stresses within the system. Exciting the second tower mode (as actually occurred in this particular case) will certainly cause certain effects on the shaft which will not be captured from any static based analysis. 488 Structural Engineering Analysis and Design Second Edition The axial force time history in an inner cable when the outer cable snaps is shown. Static Phase Convergence to New Static Equilibrium Position Outer Cable Snaps 489 Structural Engineering Analysis and Design Second Edition The time enveloped axial force within the 1D elements of the system is presented for design purposes. Of course, for completion, the time enveloped shear in 2 directions, bending about 2 axes and torsion would also have to be presented. 490 Structural Engineering Analysis and Design Second Edition 4.9.5 GNL, MNL Explicit Central FD Scheme for Newton’s Dynamic Equilibrium ODE (LS-DYNA) 4.9.5.1 Solution of Partial or Ordinary Differential Equations Using Finite Difference (FD) Schemes Finite difference mathematical methods are used to solve partial and ordinary differential equations (PDEs and ODEs) which are too complicated for exact analytical methods. Finite difference methods are thus numerical methods that are subjected to stability and accuracy requirements when solving the differential equations. The only mathematics required is the elegant Taylor’s theorem which states that for a function φ(t), φ ( t + ∆t ) = φ( t ) + ∆t ∂φ( t ) (∆t )2 ∂ 2 φ( t ) + + ... ∂t 2 ∂t 2 The expression will be exact if an infinite number of terms are taken and if ∆t is small. We can also readily state that φ ( t − ∆t ) = φ( t ) − ∆ t ∂φ( t ) (∆t )2 ∂ 2 φ( t ) + − ... ∂t 2 ∂t 2 Finite difference schemes utilize the above two expressions to reduce the PDEs or the ODEs to a set of coupled or uncoupled equations with the same number of unknowns as the number of equations so that they can be solved. A set of coupled equations will require simultaneous solution algorithms (or inversing the matrix, which of course is not performed as is computationally too intensive). A finite difference scheme, which reduces the PDEs or ODEs to a set of coupled equations, is termed an implicit scheme. In an implicit scheme, the value for a variable at a particular grid at t+∆t is related to variables at adjacent grid points for the same time level. Conversely, a set of uncoupled equations do not required any simultaneous solution algorithms. A finite difference scheme, which reduces the PDEs or ODEs to a set of uncoupled equations, is termed an explicit scheme. An explicit scheme solves for unknowns at time t+∆t expressed directly in terms of known values at time t (or before) and already known values at t+∆t. The central (finite) difference scheme subtracts and adds the two Taylor equations above to give the two expressions below for the first and second differential, both of which have an error in the order (∆t)2. ∂φ( t ) φ( t + ∆t ) − φ( t − ∆t ) 2 = + O(∆t ) ∂t 2 ∆t ∂ 2 φ( t ) ∂t 2 = φ( t + ∆ t ) − 2φ ( t ) + φ( t − ∆ t ) ( ∆t ) 2 + O (∆t ) 2 The forward (finite) difference scheme rearranges the first Taylor expression to give ∂φ( t ) φ( t + ∆t ) − φ( t ) = + O (∆t ) ∂t ∆t The backward (finite) difference scheme rearranges the second Taylor expression to give ∂φ( t ) φ( t ) − φ( t + ∆t ) = + O (∆t ) ∂t ∆t These schemes in themselves are not implicit or explicit. The application of these schemes to PDEs or ODEs will result in sets of equations that are implicit or explicit. The differential equation that concerns us is Newton’s Dynamic Equilibrium Ordinary Differential Equation. 491 Structural Engineering Analysis and Design Second Edition 4.9.5.2 Mathematical Formulation of Analysis – Explicit Central Finite Difference Scheme Newton’s Dynamic Equilibrium Ordinary Differential Equation at time t can be written as [M]{& u&( t )} + [C( t )]{u&( t )} + [K ( t )]{u ( t )} − {P( t )} = {0} or as follows Applying the central finite difference scheme ∂u ( t ) u ( t + ∆t ) − u ( t − ∆t ) 2 = + O(∆t ) ∂t 2 ∆t ∂ 2 u(t) ∂t 2 = u ( t + ∆t ) − 2 u ( t ) + u ( t − ∆t ) ( ∆t ) 2 + O (∆t ) 2 or in other notations we arrive to the finite difference expression   [M ] u (t + ∆t ) − 2u (t2) + u ( t − ∆t )  + [C(t )] u (t + ∆t ) − u (t − ∆t )  + [K ( t )]{u (t )} − {P( t )} + O(∆t )2 = {0} 2 ∆t ( ∆t )     The only unknown at time t+∆t in this expression is the displacement vector. We need to know initial values {u (t = 0)} and {u (t = −∆t)} to begin computation. However, we usually only know the initial displacement {u (t = 0)} and velocity {du/dt (t = 0)}. One method is to define a fictitious quantity {u (t = −∆t)} with the following procedure. Eliminating {u (t = ∆t)}, hence solving for {u (t = −∆t)}, in which from equilibrium conditions we can deduce Therefore, knowing the initial displacement {u (t = 0)} and velocity {du/dt (t = 0)}, we can obtain the fictitious quantity {u (t = −∆t)}. Now with {u (t = 0)} and {u (t = −∆t)} we can begin computation. Note however, the expression for {u(t)} can only be written explicitly after inverting the [M] matrix. In order to avoid a complicated [M] matrix inversion (effectively solving the then coupled simultaneous equations), the mass matrix must be diagonal. This is thus a requirement in LS-DYNA for all elements to have lumped mass formulations instead of coupled (or consistent) mass matrix formulations. This effectively maintains the explicit solution scheme. Had the mass matrix been coupled, simultaneous equations need to be solved making the solution scheme implicit. Also note that the time step may vary from time to time. Thus, in the above finite difference approximation, for completion, it must be stressed that the term 2∆t as the denominator in the velocity finite difference expression is the total time step over two steps, or the average multiplied by two. It is crucial to remember that not all the terms within the Taylor’s Expansion were utilized. In this case, the first 3 terms was utilized for the variation of displacement. This means that the displacement is parabolic, velocity is 492 Structural Engineering Analysis and Design Second Edition linear and the acceleration is constant over the time step. Hence that the displacement error in the finite difference approximation of the ODE is of the order of the square of the time step, O(∆t)2. The central finite difference solution scheme adopted in LS-DYNA is IV. Conditionally stable as long as ∆t < Tmin/π V. Second order accurate since O(∆t)2 4.9.5.3 Stability The stability of any finite difference scheme can be investigated by the von Neumann Fourier method of stability analysis. Using this method, it can be shown for this case that for stability of Newton’s undamped dynamic equilibrium ODE ∆t < 2 ω MAX For Newton’s damped dynamic equilibrium ODE, the stability condition is 2  ∆t <  1 + ζ 2 − ζ   ω MAX  Damping thus further reduces the critical time step. The time step is limited by the largest natural frequency of the structure which in turn is limited by the highest natural frequency of any individual element in the finite element mesh. The solution technique is conditionally stable, which means that the timestep must be kept small enough for the solution to have a physical meaning. Physically, the timestep size has to be less than the time taken for a sound wave to traverse the smallest deformable (i.e. non-rigid) element in the model so that a stress wave which travels through the element will cause a stress to develop within the element and not jump across it. This is because the speed of the sound wave c through the element is some function of its natural frequency. Hence, the timestep, ∆t has to be calculated for each and every element and the smallest governs the timestep for the whole analysis. Since we do not want the stress wave (at the speed of sound) to jump the element, the element must be less stiff, longer and/or of greater mass, thus of lower natural frequency. Since T=2π/ω, the conditionally stable explicit solution algorithm requires that the time step subdivide the lowest period by π for stability (for the undamped case). ∆t < 2 / ωmax ∆t < Tmin / π Hence to have a large time step: (i) (i) (ii) (iii) (iv) avoid as far as possible short, light and stiff elements make the relatively stiffer elements rigid employ mass scaling but ensure that the total mass added is not too much as to decrease the accuracy significantly; mass is added to elements so that their timestep is increased to the minimum set value; this automatic computation does not apply to spring elements, if which is the governing element, the user should manually add lumped masses to their nodes ensure limited hourglassing as distorted elements will decrease time step employ subcycling if there are relatively few small elements controlling the time step and the bulk of the elements have a stable time step at least twice that of the smallest element; subcycling divides elements into groups of timestep of ∆t, 2∆t, 4∆t, 8∆t, 16∆t, 32∆t and so on. For the Hughes-Liu (constant moment) beam and truss element, the critical time step is ∆t = L/c where c = speed of sound wave (E/ρ)0.5. This is as follows. We have said that ∆t < 2 / ωmax Now, for a truss 493 Structural Engineering Analysis and Design Second Edition ωmax = 2c/L Hence, ∆t < 2 / ωmax = L/c For the Belytschko beam (linear moment), the critical time step is given ∆t = L/c if the highest frequency is axial, but if the bending frequency is higher, then it is given by 0.5L ∆t = 3 1   c 3I  + 2 AL2  12I + AL where I is the maximum moment of inertia and A the area. For shell elements, the critical time step is ∆t = L/c where L is the characteristic length and c is given by E c= ρ1− ν2 For solid elements, the critical time step is L ∆t = Q + Q 2 + c 2 1 / 2       where Q is a function of some bulk viscosity coefficients. For elastic materials with constant bulk modulus, the speed of sound c is given by E(1 − ν ) c= ρ(1 + ν )(1 − 2ν ) The critical time step for a scalar spring is 2M 1 M 2 ∆t = 2 k (M 1 + M 2 ) ( ) { } From the critical time step equations, we can conclude that Ι. Since ∆t α ρ1/2, mass scaling is only marginally effective in increasing time step. ΙΙ. Since ∆t α L, increase the dimension of the element is very effective in increasing time step. III. Comparison of the critical time step for the truss element and the solid element shows that, for nonzero Poisson’s ratio, the solid element gives considerably smaller time steps. The critical time step for shell elements is much more comparable to that of the truss element for non-zero Poisson’s ratio. 4.9.5.4 Accuracy It is crucial to remember that not all the terms within the Taylor’s Expansion were utilized. In this case, the first 3 terms was utilized for the variation of displacement. This means that the displacement is parabolic, velocity is linear and the acceleration is constant over the time step. Hence that the displacement error in the finite difference approximation of the ODE is of the order of the square of the time step, O(∆t)2. The time step size requirement to satisfy stability is usually sufficient to satisfy accuracy requirements. It is often mentioned that for good accuracy, the time step must subdivide the lowest period of interest by 10, a condition which is usually satisfied if the lowest period is subdivided by π. The order of error generated as detailed above must however be remembered. 494 Structural Engineering Analysis and Design Second Edition 4.9.6 4.9.6.1 GNL, MNL Implicit Newmark Scheme for Newton’s Dynamic Equilibrium ODE (MSC.NASTRAN) Mathematical Formulation of Analysis – Implicit Newmark Scheme The Newmark method was proposed by Nathan Newmark and it is a general method that encompasses a family of different integration schemes including the linear acceleration and constant-average-acceleration methods. This method can be derived by considering the Taylor series expansions of the displacement and velocity at time ti+1 about ti with some remainder terms. where 0<θ1,2<1. We can now approximate the displacement and velocity using truncated Taylor series. where the terms containing β and γ represent the remainder terms in the Taylor series expansions. Since the exact values of the remainder terms are not known, β and γ are parameters to be chosen by the user to arrive at a numerical approximation. With some rearrangements of the above two equations, the Newark method comprises the following three equations With some manipulation the following equivalent static equation is obtained. where The Newmark-β method assumes some degree of contribution of acceleration from times t and t+∆t. When γ is anything other than 0.5, superfluous damping is introduced into the system. Hence it is usually taken as 0.5. β can vary from 1/6 to ½ although if γ=0.5, β has got to be greater than ¼ for unconditional stability. The general Newmark-β scheme encapsulates the following schemes. β = 0, γ = ½ the explicit central difference scheme, but the above procedure inapplicable β = 1/2, γ = ½ the implicit linear acceleration scheme β = 1/4, γ = ½ the implicit constant-average-acceleration (a.k.a. trapezoidal) scheme β = 1/6, γ = ½ the implicit linear acceleration β = 1/12, γ = ½ the implicit Fox-Goodwin method which is 4th order accurate The Newmark-β scheme is unconditionally stable as long as γ ≥ 0.5 and β ≥ 0.25 (γ + 0.5)2. In general the Newmark-β is second order accurate. 495 Structural Engineering Analysis and Design Second Edition The Wilson-θ method is an extension of the linear acceleration method, but the acceleration is assumed to be linear from time t to t+θdt. The scheme is unconditionally stable if θ ≥ 1.37. Usually θ = 1.40 is employed. When θ = 1, the scheme is equivalent to the linear acceleration method. The critical step size depends on the damping as well as the natural frequency of the structure. The values shown in the table assume that damping is zero. In general, the increase of damping increases the critical step sizes, although this effect is nullified as long as γ = 0.5. The Newmark-β (β=1/3 default) (3-point integration scheme) implicit solution scheme adopted in MSC.NASTRAN SOL 109 is IV. Unconditionally stable V. Second order accurate since O(∆t)2 The Newmark-β (β=1/3 default) (3-point integration scheme) implicit solution scheme adopted in MSC.NASTRAN SOL 129 (AUTO or TSTEP) is I. Unconditionally stable II. Second order accurate since O(∆t)2 The Newmark-β (β=1/4 default) (2-point integration scheme) implicit solution scheme adopted in MSC.NASTRAN SOL 129 (ADAPT) is I. Unconditionally stable II. Second order accurate since O(∆t)2 The recommended default SOL 129 ADAPT scheme solves using the implicit constant-average-acceleration (a.k.a. trapezoidal) scheme such that where 496 Structural Engineering Analysis and Design Second Edition where η denotes numerical damping (PARAM, NDAMP). The ADAPT (default) is used to modify the integration time step automatically (within bounds) during the analysis to respond to changes in the frequency content of the loading on TLOADi and the response natural frequency. 4.9.6.2 Stability The implicit Newmark-β scheme is unconditionally stable as long as γ ≥ 0.5 and β ≥ 0.25 (γ + 0.5)2. Hence, the time step can be as large as possible. However, the accuracy requirements will govern the size of the time step. The critical time step for Newmark-β schemes is From the above expression, we can see that when γ = 1/2, damping does not influence the critical step size. However, when γ > 1/2, the increase of damping tends to increase the critical step size. 4.9.6.3 Accuracy It is often mentioned that for good accuracy, the time step must subdivide the lowest period of interest by 10. For the purposes of illustration, lets consider the fundamental bending frequency (although in theory we should consider the higher frequencies of interest from all modes whether bending, axial or torsional) of a simply supported beam. Discretizing the beam as a lumped dynamic mass in the middle and assuming that the fundamental mode shape resembles the static deflected shape (because the p0i/Ki term is largest for the fundamental mode), and with the knowledge that the static deflection due to a unit point load on a simply supported beam is ∆1 = L3/(48EI), the unconditionally stable implicit solution algorithm requires that the time step subdivide (by at least 10 for good accuracy) the period of interest for accuracy ∆t < 2π / 10ω1 < π/5 (m/k)1/2 < π/5 (ρAL∆1)1/2 < π/5 (ρALL3/(48EI))1/2 < π/5 L2 (ρA/(48EI))1/2 A small time step is necessary for accuracy. The following should be considered for accuracy: (a) The time step should be smaller than 1/10 of the lowest natural period of interest of the system (b) The time step should be small enough to properly represent the variation of loading and capture all the significant peaks and troughs 497 Structural Engineering Analysis and Design Second Edition 4.9.7 Comparison Between Implicit and Explicit Time Integration Schemes The choice between employing an implicit or explicit time integration solution technique depends on the points listed below. These conditions are essential and must be considered for the physical problem being solved. Implicit Time Integration Explicit Time Integration Requires inversion of stiffness matrix, which for nonlinear structures changes from time to time. Hence, Does not require inversion of stiffness matrix, and the use of implicit methods for nonlinear structures stiffness matrix automatically updated at each time step. requires a Newton-type iterative approach, which is not needed in explicit methods. The cost per timestep is large The cost per time step is small Element formulation should be complex as the matrix inversion dominates the cost Element formulation should be simple as element processing dominates the cost Coarser mesh as element formulation complex Finer mesh as element formulation simple Appropriate for smaller models as the computational cost of an implicit analysis varies proportionally to the 7th power of a 3D model size. Hence the cost increase for doubling the mesh density of solid elements is x 128. Appropriate for larger models as the computational cost of an explicit analysis varies proportionally to the 4th power of a 3D model size. Hence the cost increase for doubling the mesh density of solid elements is x 16. Extremely appropriate if the model is materially linear, geometrically linear and has no contact definitions, failing which the large time step no longer enables the perfectly accurate representation of the Extremely appropriate if the model is materially highly tangent stiffness matrix over a large range of strain nonlinear, geometrically highly nonlinear and has increment. Nonlinear models can still be analyzed with contact definitions implicit schemes but the small time step requirement for accuracy (not stability) means that it is more computationally beneficial to use an explicit scheme. The solution is unconditionally stable, hence a large time step can be employed, the size of which is limited only by accuracy of the solution; The time step for an implicit analysis is usually 100 – 1000 times greater than that of an explicit analysis. The time step needs to subdivide the smallest period (highest frequency) of interest for accuracy in the model. The solution is conditionally stable, hence a small time step must be employed. The time step needs to subdivide the smallest period (highest frequency) for stability in the model. This automatically takes care of accuracy requirements, which also requires the subdivision of the smallest period. Appropriate if the physics of the problem do not Appropriate if the physics of the problem require a require a small time step, such as in stress wave small time step, such as in stress wave transmission transmission problems problems The only way to check whether the time step for accuracy in an implicit analysis is adequate is to repeat the last part of the analysis with a reduced time step and check that the results are not significantly affected. The time step in both implicit and explicit analyses is limited by the highest frequency in the structure or the lowest period. But 498 Structural Engineering Analysis and Design Second Edition the difference with implicit analysis is that since it is an unconditionally stable solution scheme, the time step is limited by the highest frequency of interest, in most instances that of only the first few initial modes of vibration. On the other hand, an explicit scheme requires that the time step subdivide the lowest period in the model as it is a conditionally stable algorithm. Thus, we are trying to minimize the largest frequency in the structure. Hence, short, stiff and light components are not computationally efficient for time integration analysis. We have seen that the choice of employing an implicit or explicit scheme depends on a lot of parameters. The fundamental difference is the size of the time step, which directly affects the computational speed. The time step in an implicit scheme is governed by accuracy conditions (∆t must subdivide smallest period of interest by 10) and not by stability conditions of which there are none. The time step in an explicit scheme is governed by stability conditions (∆t must subdivide smallest period by π) and not by the accuracy conditions (∆t must subdivide smallest period of interest by 10), which are usually automatically satisfied. As mentioned, another clear indication of whether to employ an implicit or explicit scheme is the physics of the problem. If the system is highly nonlinear (geometrically, materially and due to contact definitions), then the requirement of a small time step for accuracy (as the stiffness, damping and external force within a time step is assumed constant) usually nullifies the benefit of the unconditionally stable large time step requirement for stability of an implicit scheme. Likewise in stress propagation problems. In these circumstances, it is prudent to employ an explicit time integration scheme, which has a small time step requirement for stability anyhow. The time taken to move one time step is much smaller in an explicit scheme than an implicit scheme due to the requirement of matrix inversion or simultaneous equation solving algorithms in the latter. 499 Structural Engineering Analysis and Design Second Edition 4.9.8 MSC.NASTRAN Decks 4.9.8.1 GNL, MNL Direct Forced (Implicit) Transient Response Analysis All cards applicable to SOL 109 are also applicable to SOL 129. $ EXECUTIVE CONTROL SECTION SOL 129 $ CASE CONTROL SECTION $ Sets defining grid ids or element ids SET < Number > = 1 THRU 100, 211, 343, < etc > $ Grid output of displacement, velocity and acceleration with time $ SORT1 lists the results by time whilst SORT2 lists the results by grid id DISPLACEMENT(,) = ALL/ VELOCITY(,) = ALL/ ACCELERATION(,) = ALL/ $ Grid output of applied load vector OLOAD(,) = ALL/ $ Grid output of d-set displacement, velocity and acceleration SDISPLACEMENT(,) = ALL/ SVELOCITY(,) = ALL/ SACCELERATION(,) = ALL/ $ Grid output of SPC forces SPCFORCES(,) = ALL/ $ Element output of force, stress and strain ELFORCE(,) = ALL/ ELSTRESS(,) = ALL/ STRAIN(,) = ALL/ NLLOAD(PLOT) SUBCASE 1 SPC = < ID of SPC Cards Defined in Bulk Data > DLOAD = < ID OF TLOAD1 or TLOAD2 > NONLINEAR = < ID OF NOLINi > TSTEPNL = < ID OF TSTEPNL > SUBCASE 2 SPC = < ID of SPC Cards Defined in Bulk Data > DLOAD = < ID OF TLOAD1 or TLOAD2 > NONLINEAR = < ID OF NOLINi > TSTEPNL = < ID OF TSTEPNL > $ XY plot output OUTPUT(XYPLOT) XYPUNCH RESPONSE /() XYPUNCH RESPONSE /() $ BULK DATA PARAM, PARAM, PARAM, PARAM, PARAM, AUTOSPC, NO FOLLOWK, YES LGDISP, 1 LANGLE, 2 K6ROT, 100 $ $ $ $ $ AUTOSPC NO By Default Includes Follower Force Stiffness Includes Large Displacement Effects i.e. [T] not constant Rotation Vector Approach for Large Rotations Shell normal rotation restrained in nonlinear analysis Mass-less DOFs should be avoided in SOL 129. The time step should be based on capturing the maximum frequency of interest. In linear analysis (SOL 109 and SOL 112) it is recommended that the time step, DT be a tenth of the period representing the highest frequency of interest (i.e. if 100Hz, then DT should be 0.001s) and that 500 Structural Engineering Analysis and Design Second Edition DT should be small enough to accurately capture the highest frequency content of the excitation (i.e. if 1000Hz, then DT should be 0.001s or less). In nonlinear analysis SOL 129, if NOLINi is incorporated, DT should be 1/5 to 1/10 the size described above since NOLINi puts the structure out of equilibrium by one time step, so a very small integration time step is required to minimize this limitation. The TSTEPNL bulk data entry is as follows. Unlike linear analyses schemes, nonlinear analysis schemes (SOL 106 and SOL 129) employ subcases on an incremental basis, instead of separate load cases and boundary conditions. For SOL 129, the bulk data loads and prescribed motions are measured from the initial configuration at time zero. The following can be performed with multiple subcases: (i) (ii) (iii) Loads can be changed SPC cannot be changed. However, the change in boundary condition can more often than not be defined with prescribed motion load curves The initial time step size DT can be changed The duration of the analysis is the number of time steps NDT times the time step size DT, which in general varies. NO is the time step interval for output. In this NONLINEAR TIME DOMAIN solution, the static response must be added to the dynamic response if the dynamic analysis is performed about the initial undeflected (by the static loads) state with only the dynamic loads applied, hence causing the dynamic response to be measured relative to the static equilibrium position. Hence, the total response = the dynamic response + the static response to static loads. Time domain dynamic excitation functions should always be applied from the amplitude of 0.0 (and realistically de-ramped to 0.0 as well). This is because inherently, the dynamic excitation function has to be extrapolated within the analysis code to be from 0.0. Hence, that initial jolt should better be representative of reality irrespective of whether load excitations or enforced motion is being applied. Alternatively, in this NONLINEAR TIME DOMAIN solution, if the dynamic analysis is performed with the deflected static shape as initial input and the static loads maintained throughout the dynamic excitations, the total or absolute response (static and dynamic) is obtained straight away from the dynamic analysis. Hence total response = dynamic response (which already includes the static response to static loads). Of course, if the transient dynamic analysis follows a static analysis (by say SOL 101, SOL 106, implicit dynamic relaxation by SOL 129 or explicit dynamic relaxation), then the dynamic excitation function should be ramped up from the static amplitude and not from 0.0 (and realistically de-ramped to the static load as well), so that again there would be no jolt unrepresentative of reality. 4.9.8.1.1 Time Step and Stiffness Update Strategy (ADAPT with ADJUST, MSTEP, RB and MAXR, AUTO, TSTEP with KSTEP) The load is divided up into time steps. Each time step is then divided into iteration steps. METHOD specifies the method for controlling time step and stiffness updates, whether ADAPT (default), AUTO or TSTEP. The ADAPT (default) is used to modify the integration time step automatically (within bounds) during the analysis to respond to changes in the frequency content of the loading on TLOADi and the response natural frequency. However, it may force the solution to solve for unnecessary high frequency modes. DT is used as an initial time step estimate. ADJUST controls the automatic time stepping, by default 5. If ADJUST = 0, then the automatic adjustment is deactivated. If ADJUST > 0, the time increment is continually adjusted for the first few steps until a 501 Structural Engineering Analysis and Design Second Edition good value of DT is obtained. After this initial adjustment, the time increment is adjusted every ADJUST-th time step only. MSTEP and RB are used to adjust the time increment during analysis. MSTEP is the number of steps to obtain the dominant period response and RB defines bounds for maintaining the same time step for the stepping function during the adaptive process, default 0.75. The recommended value of MSTEP for nearly linear problems is 20. A larger value (e.g., 40) is required for highly nonlinear problems. By default, the program automatically computes the value of MSTEP based on the changes in the stiffness. The time increment adjustment is based on the number of time steps desired to capture the dominant frequency response accurately. The time increment is adjusted as follows. where MAXR is the maximum ratio for the adjusted incremental time relative to DT allowed for time step adjustment, by default 16. MAXR is used to define the upper and lower bounds for adjusted time step size as follows. ADAPT is the average acceleration scheme with β = 0.25 and can be made to behave similarly to AUTO and TSTEP using MAXR set to 1.0 to prevent time step changes and possibly also set KSTEP to 1. AUTO is analogous to AUTO in SOL 106. Time step is constant with AUTO. TSTEP with KSTEP is analogous to ITER with KSTEP in SOL 106. Time step is constant with TSTEP. The METHOD field selects an option for direct time integration and the stiffness matrix update strategies among ADAPT, AUTO and TSTEP. If the AUTO option is selected, MSC.Nastran automatically updates the stiffness matrix to improve convergence while the KSTEP value is ignored. If the TSTEP option is selected, MSC.Nastran updates the stiffness matrix every KSTEP-th increment of time. If the ADAPT option is selected, MSC.Nastran automatically adjusts the incremental time and uses the bisection algorithm in case of divergence. During the bisection process in the ADAPT option, stiffness is updated at every KSTEP-th successful bisection. The ADAPT method allows linear transient analysis, but AUTO or TSTEP will abort the run if the model does not have any data representing nonlinearity. The stiffness matrix is always updated for a new subcase or restart, irrespective of the option selected. 4.9.8.1.2 Convergence Acceleration Techniques (Quasi-Newton MAXQN, Line Search using MAXLS, Bisection using MAXITER, RTOLB, MAXBIS and MAXDIV) Quasi-Newton updates and line search is as SOL 106. In SOL 129, the default for MAXQN is 10 and MAXLS is 2. MAXITER specifies the limit on number of iterations for each time step, 10 by default. The sign of MAXITER provides a control over the ultimate recourse (reiteration) in case of failure in convergence or bisection. If the MAXITER is negative, the analysis is terminated when the divergence condition is encountered twice during the same time step or the solution diverges for five consecutive time steps. If MAXITER is positive, the program computes the best attainable solution and continues the analysis on second divergence. If the solution does not converge at MAXITER iterations, the time step is bisected and the analysis is repeated. Bisection is also activated if RTOLB, by default 20.0 is exceeded. RTOLB is the maximum value of incremental rotation (in degrees) 502 Structural Engineering Analysis and Design Second Edition allowed per iteration before bisection is activated. MAXBIS specifies the maximum number of bisections for each time step, 5 by default. If MAXBIS is positive and the solution does not converge after MAXBIS bisections, the best solution is computed and the analysis is continued to the next time step. If MAXBIS is negative and the solution does not converge in |MAXBIS| bisection, the analysis is terminated. MAXDIV provides control over diverging solutions, default 2. Depending on the rate of divergence, the number of diverging solutions (NDIV) is incremented by 1 or 2. The solution is assumed to diverge when NDIV reaches MAXDIV during the iteration. If the bisection option is used (allowed MAXBIS times) the time step is bisected upon divergence. Otherwise, the solution for the time step is repeated with a new stiffness based on the converged state at the beginning of the time step. If NDIV reaches MAXDIV again within the same time step, the analysis is terminated. The number of iterations for a time step is limited to MAXITER. If the solution does not converge in MAXITER iterations, the process is treated as a divergent process; i.e., either a bisection or stiffness matrix update takes place based on the value of MAXBIS. The sign of MAXITER provides a control over reiteration in case of failure in convergence or bisection. If MAXITER is negative, the analysis is terminated when the divergence condition is encountered twice during the same time step or the solution diverges for five consecutive time steps. If MAXITER is positive, MSC.Nastran computes the best attainable solution and continues the analysis. The MAXDIV field provides control over diverging solutions. Depending on the rate of divergence, the number of diverging solutions (NDIV) is incremented by 1 or 2. The solution is assumed to be divergent when NDIV reaches MAXDIV during the iteration. If the bisection option is used with the ADAPT method, the time step is bisected upon divergence. Otherwise, the solution for the time step is repeated with a new stiffness based on the converged state at the beginning of the time step. If NDIV reaches MAXDIV twice within the same time step, the analysis is terminated with a fatal message. 4.9.8.1.3 Convergence Criteria (CONV, EPSU, EPSP, EPSW) CONV specifies the flags to select convergence criteria, UPW or any combination, note default PW. EPSU is the error tolerance for displacement error (U) convergence criteria, 1.0E-2 by default. EPSP is the error tolerance for load equilibrium error (P) convergence criteria, 1.0E-3 by default. EPSW is the error tolerance for work error (W) convergence criteria, 1.0E-6 by default. These correspond to the very high tolerance, PARAM, NLTOL, 0 unlike SOL 106 which had engineering tolerance levels PARAM, NLTOL, 2. 4.9.8.1.4 Nonlinear Transient Load Nonlinear transient loads, which are functions of the displacement and/or velocity of the response, can be specified using NOLINi entries. 4.9.8.1.5 Nonlinear Finite Elements, Nonlinear Material Definitions and Nonlinear Contact Interface The nonlinear finite elements, the nonlinear material definitions and the nonlinear contact interface are as defined in the nonlinear static analysis SOL 106 section. 503 Structural Engineering Analysis and Design Second Edition 4.9.8.2 Nonlinear Static Analysis and Nonlinear Transient Analysis Subcases can be employed to change the method of analysis from SOL 106 to SOL 129. 4.9.8.3 Restart From Nonlinear Static Analysis SOL 106 Into Nonlinear Transient Analysis SOL 129 Restarts are allowed from end of subcases. A LOOPID is created after each converged load increment in static analysis and at the end of each converged subcase in nonlinear transient analysis. Only LOOPIDs written to the database and identified as such in the printed output can be used for a restart. $ BULK DATA PARAM, SLOOPID, L $ Load Step ID, L at the End of a Subcase of the SOL 106 Run The initial transient loads should be identical to the static loads at the restart state. This is to ensure no sudden jump in load. The changes allowed in model are (i) Boundary conditions, i.e. SPC (ii) Direct input matrices (iii) Mass (iv) Damping Note that when restarting a transient analysis from a static analysis, the static loads which have been applied must be maintained throughout the transient phase. 4.9.8.4 Restart From Nonlinear Transient Analysis SOL 129 Into Nonlinear Transient Analysis SOL 129 Restarts are allowed from end of subcases. $ FMS RESTART $ BULK DATA PARAM, LOOPID, L PARAM, STIME, T $ Loop Number on Printout, L $ Starting Value of Time, T Note that when restarting a transient analysis from a static analysis (whether a Newton-Raphson nonlinear static analysis or dynamic relaxation), the static loads which have been applied must be maintained throughout the transient phase. Hence, when a transient phase dynamic analysis follows a dynamic relaxation analysis, it is prudent to define two curves for the static loads or prescribed motions, one ramped from zero to the static value in the dynamic relaxation phase and the other maintained at the same static throughout the transient dynamic analysis phase. 504 Structural Engineering Analysis and Design Second Edition 4.9.8.5 Implicit Nonlinear (Static and) Dynamic Analysis SOL 400 SOL 400 replaces SOL 106 and SOL 129 adding MSC.Marc’s 3D contact routines, large rotation of rigid bodies and additional types of rigid mechanisms directly inside MSC.Nastran. 4.9.8.6 Implicit Nonlinear (Static and) Dynamic Analysis SOL 600 SOL 600 is the MSC.Marc implicit nonlinear static and dynamic analysis solver within MSC.NASTRAN. 4.9.8.7 Explicit Nonlinear Dynamic Analysis SOL 700 SOL 700 is the LS-DYNA explicit nonlinear dynamic analysis solver within MSC.NASTRAN. 505 Structural Engineering Analysis and Design Second Edition 4.9.9 4.9.9.1 LS-DYNA Decks GNL, MNL Direct Forced (Explicit) Transient Response Analysis To specify termination time of the explicit dynamic analysis *CONTROL_TERMINATION Termination Time Limit Termination Cycle Limit Termination Min Time Step Size Limit Termination Energy Ratio Limit To set structural timestep size control and invoke mass scaling *CONTROL_TIMESTEP Min Time Initial Time Factor For Shell Min Step For Basis Step Time Step Time Step Mass Scaling Termination Change in Total Mass From Mass Scaling Maximum Time Step Curve Erosion Flag Limit Mass Scaling To enable subcycling *CONTROL_SUBCYCLE To specify user-defined boundary conditions for the transient phase, *LOAD_NODE_ (HM: forces, moments) *SET_NODE *DEFINE_CURVE with SIDR = 0 for transient phase *LOAD_BEAM_ *SET_BEAM *DEFINE_CURVE with SIDR = 0 for transient phase *LOAD_SHELL_ (HM: pressure ShellPres) *SET_SHELL *DEFINE_CURVE with SIDR = 0 for transient phase *LOAD_RIGID_BODY *DEFINE_CURVE with SIDR = 0 for transient phase *LOAD_SEGMENT_ (HM: pressure SegmentPre) *SET_SEGMENT *DEFINE_CURVE with SIDR = 0 for transient phase To apply automatically computed gravitational loads, noting that by d-Alembert’s principle, applying accelerations in a certain direction results in inertial loads acting in the opposite direction. Hence, a downward gravity is applied as an upward acceleration. *LOAD_BODY_Z with sf = 9.81 ms-2 *DEFINE_CURVE with SIDR = 0 for transient phase Do not apply gravity loads on soil elements because the in-situ measured soil properties already take into account its stiffness with gravity applied. 506 Structural Engineering Analysis and Design Second Edition To prescribe displacements, velocity or accelerations (as in seismic analysis) on a node, on a set of nodes, on a rigid body in the global axes system or on a rigid body in the rigid body local axes system, *BOUNDARY_PRESCRIBED_MOTION_ (HM: velocities prcrbVel or HM: accels) Velocity, Load Curve NID, NSID, Acceleration or VID DEATH BIRTH DOF LCID Scale Factor or PART ID Displacement SF VAD The vector ID, VID is used to specify a direction vector if imposed motion not in global axes system. DEATH and BIRTH can be used to specify deactivation and activation times of the imposed motion during the analysis. *SET_NODE_LIST DA1 NSID NID NID NID NID DA2 NID NID DA3 NID NID DA4 NID … NID … NID … NID … *DEFINE_CURVE SFA SFO OFFA OFFO DATTYP LCID SIDR Abscissa Values Ordinate Values Abscissa Values Ordinate Values … … SIDR defines whether the curve is valid for the transient phase, stress initialization phase or both. Here obviously, SIDR = 0. Having said that, for every transient pair of *BOUNDARY_PRESCRIBED_MOTION and *DEFINE_CURVE cards defined, it is generally necessary to define two corresponding cards that is valid for the stress initialization (dynamic relaxation) phase if dynamic relaxation is activated. For instance, if the earthquake acceleration time histories are to be applied in the transient phase, it is necessary to define zero velocity prescribed boundary conditions for the dynamic relaxation phase so that the structure is supported. The BOUNDARY_PRESCRIBED_MOTION card is useful to change boundary conditions during an analysis. *DEFINE_VECTOR if DOF not global i.e. VID defined VID XTail YTail ZTail Xhead Yhead To prescribe initial conditions *INITIAL_VELOCITY_ (HM: velocities initVel) *SET_NODE or, *PART_INERTIA or, *CONSTRAINED_NODAL_RIGID_BODY_INERTIA 507 ZHead Structural Engineering Analysis and Design Second Edition 4.9.10 Hand Methods Verification 4.9.10.1 Determination of Displacement Response Time History by Solving the SDOF Nonlinear (in Stiffness, Damping and Displacement) Equation of Motion ODE for Deterministic Time Domain Loading With/Without Initial Conditions by Implicit Newmark-β Time Integration Schemes Nonlinear time domain hand methods are capable of analyzing: - SDOF or Single-Modal Response to Deterministic Non-Periodic Short Duration Impulse and Hence Random Non-Stationary Short Duration Impulse by Enveloping Deterministic Responses Multi-modal nonlinear response cannot be performed because the superposition of nonlinear modal responses is not strictly valid for nonlinear systems where the physical coordinates (which includes all modes together) responds nonlinearly. Nonlinear analysis can be performed by the implicit Newmark-β method (constant acceleration, linear acceleration etc.) or the implicit Wilson-θ method. Since hand computations are limited to SDOF system, all the algorithms are explicit as there is no need for matrix inversion (or solving of simultaneous equations). The loading is divided into a sequence of time intervals. The response is evaluated at successive increments ∆t of time, usually taken of equal lengths of time for computational convenience. At the beginning of each interval, the condition of dynamic equilibrium is established. Then, the response for the time increment ∆t is evaluated approximately on the basis that the coefficients k and c remain constant during the interval ∆t. The non-linear characteristics of these coefficients are considered in the analysis be re-evaluating these coefficients at the beginning of each time increment. The response is then obtained using the displacement and velocity calculated at the end of the time interval as the initial conditions for the next time step. Hence, basically the equation of motion (non-linear in that k and c changes at every time interval but constant within the interval) is solved for at each and every time step, the initial conditions at each time step being the displacement and velocity calculated at the end of the previous time interval. Also, the P(t) is unique for each and every time interval. m& u&( t ) p(t) k(t)u(t) m u(t) c(t)u&(t) The general nonlinear Newton’s dynamic equation of motion at time ti can be written as m& u&i + c i u&i + k i u i = Pi The incremental form of the equation of motion is then m∆& u&i + c i ∆u&i + k i ∆u i = ∆Pi The choice of the time integration scheme depends on the acceleration variation function across the time step. We shall describe the Newmark-β method, which includes the constant acceleration and linear acceleration schemes within its formulation. The Newmark-β method states the Newmark equations as 1 ∆u&i = & u&i ∆t + γ∆& u&i ∆t and ∆u i = u&i ∆t + & u&i ∆t 2 + β∆& u&i ∆t 2 2 When γ is anything other than 0.5, superfluous damping is introduced into the system. Hence it is usually taken as γ = 0.5. β can vary from 1/6 to ½ but is unconditionally stable only as long as β ≥ 0.25 (γ + 0.5)2. When β is ¼, the Newmark equations can be obtained from assuming the constant acceleration method (unconditionally stable) & u&( t ) = 1 (& u&i + & u&i +1 ) 2 508 Structural Engineering Analysis and Design Second Edition and when β is 1/6, the Newmark equations can be obtained from assuming the linear acceleration method (conditional stability although implicit! note β ≥ 0.25 (γ + 0.5)2 for unconditional stability) & u&( t ) = & u&i + ∆& u&i (t − t i ) ∆t On rearranging the Newmark equations, u&i = ∆& ∆u i β(∆t ) 2 It is wise to choose γ = 0.5 No superfluous damping 0.25 < β < 0.5 Unconditionally stable u& 1 & − i − u&i β(∆t ) 2β  ∆u i  u& 1 & ∆u&i = & u&i ∆t + γ − i − u&i  ∆t 2 β(∆t ) 2β   β(∆t )  γ γ  γ & = ∆u i + 1 − u&i ∆t − u&i β(∆t ) 2β  β  Replacing these rearranged Newmark equations into the incremental form of the equation of motion to yield only ∆ui as the unknown. This will be rearranged for ∆ui.  ∆u i   γ u&  1 γ  γ  & & m − i − u&i  + c i  ∆u i + 1 − u&i ∆t − u&i  + k i ∆u i = ∆Pi 2 β(∆t ) 2β  2β  β    β(∆t )  β(∆t ) This can thus be implemented on a spreadsheet and looped over numerous time steps. The procedure is described as follows: (a) Choose appropriate time step ∆t (b) Establish initial conditions noting that u(t) is relative to the static equilibrium position u 0 , u&0 , & u&0 For i = 0 To Number of Increments (c) Calculate incremental displacement from m  γ    m γ  ∆Pi +  + ∆t  − 1c i & u&i +  + c i  u&i ( ) 2 2 β ∆ t β β β       ∆u i = 1 γ m+ ci + k i 2 β(∆t ) β(∆t ) (d) Calculate incremental velocity from (e)  γ γ  γ & ∆u i + 1 − u&i ∆t − u&i β(∆t ) 2 β β   Compute displacement and velocity at new time i + 1 as ∆u&i = u i +1 = u i + ∆u i u&i +1 = u&i + ∆u&i (f) Compute the acceleration at the new time i + 1 directly from differential equation noting that c and k may vary according to some condition on the velocity or displacement & u&i +1 = 1 (Pi +1 − c i +1 u&i +1 − k i +1 u i +1 ) m Next i 509 Structural Engineering Analysis and Design Second Edition 5 Advanced Applications of Methods of Static and Dynamic Analyses 5.1 Earthquake Induced Vibrations 5.1.1 5.1.1.1 Engineering Seismology Seismic Risk Seismic Risk = Hazard x Exposure x Vulnerability x Specific Loss (assess) (assess) (reduce) (reduce) Hazard is the probability of a potentially damaging earthquake effect occurring at the site of a construction within its design life; It involves the level of seismic effect and the corresponding probability of occurrence. Hazard is to be assessed by seismic hazard assessment. Exposure is the concentration of human, commercial and industrial activity at a site subject to earthquake effects. Vulnerability is the level of damage that will be experienced by a structure when exposed to a particular earthquake effect; Vulnerability is to be reduced by sound structural earthquake engineering. Specific loss is the cost of restoring a structure to its original condition as a proportion of the cost of demolition and rebuilding a similar structure; Specific loss must be minimised by sound structural earthquake engineering. The Kobe earthquake of magnitude MS = 7.0 on 17 January 1995 in Japan left 5,420 people without life and caused US$150 billion, the largest ever single loss from an earthquake. 5.1.1.2 Physics of the Earth Earth’s radius = 6,370 km so an arc on the surface of the planet subtending an angle of 1° at the centre has a length of 111km. Crust is composed of brittle granitic and basaltic rocks. Crust thickness = 10–15 km in oceanic areas and 30–50 km in continental areas. Lithosphere = Outer part of mantle and the crust; It has a thickness of about 60km in oceanic regions and 100km in continental regions; The lithosphere is the only part of the earth that exhibits brittle characteristics and hence the only part where earthquake can occur. Focal depths greater than the thickness of the lithosphere occur in the subduction zones where the lithosphere descends into the mantle. 5.1.1.3 Plate Tectonics The convection currents in the asthenosphere (soft layer of about 200km in thickness below lithosphere) cause the 1-5cm/year movement of the lithosphere, which is divided into 12 major tectonic plates. The movement can be catagorised into: (a) sea-floor spreading at mid-oceanic ridges as in the Atlantic Ocean (b) subduction as in the Pacific Coast of Central and South America (c) transcursion as along the San Andreas fault in California 5.1.1.4 Global Seismicity The global distribution of earthquakes: (a) Interplate (i) circum-Pacific belt 75% (ii) Alpide-Asiatic belt 22% (iii) mid-oceanic ridges 2% (b) Intraplate (i) Japan (significant tectonic deformation) (ii) Australia, Northwest Europe, Brazil (cause not well understood) 510 Structural Engineering Analysis and Design Second Edition 5.1.1.5 Mechanism of Earthquakes: Elastic Rebound E σ O 5.1.1.6 Path: OBD = Buildup of stresses EB = Elastic Rebound B D C F ε Energy: OEF = Energy in crust before earthquake EBD = Stored elastic energy ES released through elastic waves (P-waves and S-waves) in the elastic rebound mechanism BDCF = Heat loss and inelastic deformation of the fault face OBC = Remaining energy Fault Rupture Classification Dip, δ (0° < δ ≤ 90°) Elevation View Hanging Wall (above fault plane and at the side of the dip on plan) Foot Wall (below fault plane) Strike, φ (0° ≤ φ ≤ 360°) (Clockwise from North measured to the fault dipping to the right of observer, i.e. the hanging wall on the right) Here φ ≈ 315°. Plan View Fault Plane View Rake or slip, λ (-180° ≤ λ ≤ +180°) • measured in plane of fault • measured from strike line • measured positive upwards λ = 0° (left-lateral) λ = ±180° (right-lateral) λ = +90° (reverse) λ = -90° (normal) Rupture Mechanism: (a) Horizontal strike-slip (i) Right-lateral (ii) Left-lateral (b) Vertical dip-slip (i) Normal fault (tension, hanging wall below ground level) (ii) Reverse fault (compression, hanging wall above ground level) (c) Oblique (dip and strike-slip) 511 Structural Engineering Analysis and Design Second Edition 5.1.1.7 Seismic Waves Seismic Waves Body Waves Surface Waves • • • Due directly to source of earthquake Faster than surface waves; Both VP and VS = function (elastic properties) where the stiffer the elastic medium the faster P-Wave (Primary Wave) S-Wave (Secondary Wave) • Compression Wave • Longitudinal Wave (particle motion parallel to propagation) • VP > VS; VP ~ 9 km/s VS ~ 5 km/s E(1 − ν) VP = ρ(1 + ν )(1 − 2ν) 5.1.1.8 • The reflection of P- and S-waves at the surface back to the crust sets up a disturbance in the surface which then propagates along the surface; Since they are not radiated from the earthquake, they exist at some distance from hypocentre Slower than body waves; Both VLOVE and VRAYLEIGH = function (elastic properties, wavelength) Love Wave Rayleigh Wave • Shear Wave Transverse Wave (particle motion transverse to propagation) • VP > VS; VP ~ 9 km/s VS ~ 5 km/s E G VS = = 2ρ(1 + ν) ρ • • • Horizontally polarised Vertically polarised like sea waves; but unlike sea waves, the particles under the waves travel in the opposite sense Accelerographs and Seismographs Characteristics Seismographs Accelerographs Motion Recorded Displacement / Velocity versus time Short period seismographs detect P- and Swaves Acceleration versus time Vertical long-period seismographs detect Three components, namely 2 horizontal and Rayleigh waves 1 vertical records Horizontal long-period seismographs detect Love waves Date of invention 1890 1932 Natural Period 1-20 seconds or longer (Short period and long-period) < 0.05 seconds Installation Location Far-field Near-field (close to earthquake) Operation Continuous (will pick up earthquake instantly) Standby, triggered by shaking (will not pick up earthquake instantly) Film Cartridge Speed 1 inch/minute 1 cm/second Use of records Seismology Engineering 512 Structural Engineering Analysis and Design Second Edition 5.1.1.9 Earthquake Location Parameters Parameters to define earthquake location: (i) Epicentre N, E ; Errors of the order of 5km (ii) Focal depth, h0 (km); Errors of the order 10km (iii) Origin time t0 (GMT) 5.1.1.10 Estimation of Location of Focus or Epicentre (i) Local shallow earthquakes (assuming constant velocity of waves, shallow depth i.e. DFOCUS ~ DEPICENTRE & no earth curvature)  V V  Distance of hypocentre (focus) from station, D FOCUS =  P S δT  VP − VS  Three stations’ records of DFOCUS are necessary to estimate the location of the focus or epicentre. (ii) Non-local earthquakes Use travel-time curves. By inputting the difference in travel times, δT between two phases, we can obtain the epicentral distance ∆° in degrees (x 111km to change to km) for any particular focal depth. 5.1.1.11 Estimation of Focal Depth (i) From visual inspection of the seismogram, deep earthquakes have weak surface waves; Shallow waves are a clear indication of a shallow focus. For deep earthquakes use depth phases (pP, sS, etc) (ii) If all else fails, assign arbitrary value of 10km or 33km 5.1.1.12 Estimation of Time of Earthquake Occurrence Input: Absolute time that the first earthquake wave reaches station, AT Distance from station to epicentre, D Focal depth, h Depth of topmost crust layer, d1 Compute: Velocity at the topmost crust layer of d1, V1 Velocity at the second crust layer, V2 Using Snell’s Law, compute iC sin i C sin 90° sin i sin r = , hence = V1 V2 V1 V2 Output: The travel time from focus to station is the lesser time in the following phases: Tg = T* = D2 + h2 V1 d1 (d − h ) D − (d 1 − h ) tan i C − d 1 tan i C + 1 + V1 cos i C V1 cos i C V2 Hence, the absolute time of earthquake = AT – travel time 513 Structural Engineering Analysis and Design Second Edition 5.1.1.13 Earthquake Magnitude (a) Moment Magnitude, MW based on Seismic Moment M0 Proportional to the actual rupture slip displacement size of the earthquake, U(m) Seismic Moment, M0 = measures the size of an earthquake rupture = work done in rupturing the fault = µAU Nm (~ 1015 – 1030) where the rigidity of the crust = µ ~ 3 x 1010 (Nm-2) displacement = U ~ 10-4 of rupture length of large earthquakes (m) area = A (m2) Moment Magnitude, MW = (2/3)log10(M0) – 10.7 Wells and Coppersmith (1994) proposed an equation to estimate the earthquake potential of a fault of a given length, namely, where SRL is the surface rupture length in kilometers and This based on the fact that rupture length grows exponentially with magnitude. Note that the elastic energy released grows exponentially with magnitude log10(ES) = 11.8 + 1.5MW where E is measured in ergs. A unit increase in magnitude corresponds to a 101.5 or 32-fold increase in seismic energy. Energy release from a M7 event is 1000 times greater than that from a M5 event. An observation is that ES / Volume ~ constant. (b) Richter’s Local Magnitude, ML recalibrating for specific area Proportional to the S-P interval δt and maximum trace amplitude A Richter’s Local Magnitude, ML from nomogram inputting δt and maximum trace amplitude A (mm), or Richter’s Local Magnitude, ML = log (A) – log (A0) of Richter’s tables inputting maximum amplitudes A (mm) and epicentral distance from station, ∆ (km). (c) Teleseismic Magnitude Scales, MS and mb Proportional to the maximum ratio of ground amplitude A (µm) to period of ground motion T (s) and hence independent of the type of seismograph A Surface wave magnitude, M S = log  + 1.66 log( ∆°) + 3.3 (using long - period instruments)  T  MAX A Body wave magnitude, m b = log  + Q( ∆, h ) (using short - period instruments)  T  MAX 514 Structural Engineering Analysis and Design Second Edition Moment Magnitude, MW Local Magnitude, ML Teleseismic Magnitudes MS & mb Does not saturate at large earthquakes Saturates at large earthquakes Saturates at large earthquakes Saturation refers to the fact that beyond a certain level, an increase in seismic energy release does not produce a corresponding increase in magnitude. This happens because the scales are based on readings of waves in a limited period range (determined by the characteristics of the instrument) and as the size of the earthquake source grows the additional energy release results in waves of larger period rather than increasing the amplitude of shorter period radiation. Some major earthquakes of the 20th century are presented. The 1989 Loma Prieta earthquake resulted in about 7 billion dollars in damage, not accounting for the loss of business opportunities. The total financial loss induced in the 1994 Northridge earthquake is estimated to be over 10 billion dollars. 515 Structural Engineering Analysis and Design Second Edition 5.1.1.14 Evaluation of Regional Seismicity (a) The maximum credible earthquake MMAX is first found from either (i) the maximum length of fault rupture that could physically occur log (L) = 0.7MS – 3.24 etc… (ii) MMAX = MMAX KNOWN TO OCCUR + ∆M (b) It is found that a linear relationship exists between frequency and magnitude, log (N) = a – b.M (Recurrence relationship by Gutenberg & Richter, 1954) N = number of earthquakes per year with magnitude ≥ M a = level of earthquake activity b = relative values of small and large earthquakes or brittleness of crust Putting M = MMAX, we can compute N. (c) Return Period, T = 1/N Log N Due to fact that small earthquakes not always detected, i.e. incomplete catalougue ∆b ∆a M ∆a due to saturation of scale at high M ∆b due to period of observation being too short in comparison to the return period of large earthquake 5.1.1.15 Intensity Intensity is an index related to the strength of the ground shaking and is not a measure parameter. Intensity III limit of perceptibility Intensity VII threshold of damage to structures Intensity VIII threshold of damage to engineered structures Intensity X realistic upper bound Intensity worked out by taking the modal value of an intensity histogram. 5.1.1.16 Characterisation of Strong Motion Spectral Acceleration Horizontal and vertical Peak Ground Acceleration (PGA) is the most widely used parameter although it really represents the damage for only stiff structures since damage of a structure is also a function of its period. Peak Ground Acceleration T 516 Structural Engineering Analysis and Design Second Edition Other parameters such as cycles of motion, frequency of motion and duration not taken into account. PGA also does not correlate well with earthquake damage, except for stiff structures such as 1 storey brick buildings. The strong ground motion can also be characterised by the peak values of velocity and displacement obtained by the integration of the earthquake time-history. PGA correlates well with intensity; for damaging motion (intensity VIII), we find PGA ≥ 0.2g. A widely used measure of damage potential is the energy in an accelerogram known as the Arias intensity. IA = π 2g ∫ T 0 a 2 ( t )dt 5.1.1.17 Attenuation Relationship PGA = b1e b 2M d − b3 e − b 4d The coefficients are determined by regression analysis on a database of accelerograms’ PGA and their associated magnitudes and distances. PGV and PGD poor because the integration of acceleration time history heavily influenced by the errors associated with analogue accelograms and the processing procedures (filters) that are applied to the records to compensate for them. Also, the integration assumes initial values of zero for velocity and displacement although for analogue recordings, the first readings are lost and hence, this may not be the case. Small errors in baseline estimation of acceleration cause great errors in velocity and displacement. 517 Structural Engineering Analysis and Design Second Edition 5.1.1.18 Seismic Hazard Evaluation Procedure: Seismic Hazard Curves and Seismic Hazard Maps The objective of seismic hazard assessment is to determine the probability of exceedance of a particular level of PGA at the site under consideration. (a) Seismic hazard curves are produced for a particular point or site: (i) Choose design life-span L for structure, say 50 years (ii) Determine seismic source points, I (seismic source lines and seismic source areas or zones could be converted to a number of seismic source points). Seismic source zones are delimited from catalogues of historical earthquakes. (iii) For each earthquake source i, determine MiMAX and hence PGAiMAX For each source i determine MiMAX knowing MS α log(rupture length) and catalogues of historical earthquakes using attenuation log(PGA) = c1 + c2M – c3log(d2 + h02)1/2 – c4(d2 + h02)1/2 compute PGAiMAX End For (iv) Determine LARGEST(PGAiMAX) (v) Choose a PGA ≤ LARGEST(PGAiMAX) and compute Mi for each source For each source i using attenuation log(PGA) = c1 + c2M – c3log(d2 + h02)1/2 – c4(d2 + h02)1/2 compute Mi End For Note that PGA of 0.2g corresponds to Intensity VIII that causes structural damage (vi) Compute annual frequencies Ni from recurrence relationships particular to each source For each source i log(Ni) = a – bMi , parameters obtained from catalogues of instrumental seismicity End For T If Mi > MiMAX then put Ni = 0 (vii) Compute percentage of probability of exceedance, q q i =i −L ∑ Ni PGA q = 1 − e i =1 (based on Poisson probability model) PGA (viii) Compute return period T T = 1 / ΣN (ix) Plot a point on the seismic hazard curves q vs PGA and T vs PGA (x) Loop to (iv) until complete plot of seismic hazard curves q vs PGA and T vs PGA is obtained (b) Hazard map showing the contours of PGA for a site with a specific probability of exceedance q or a certain return period T is obtained by drawing a hazard curve at numerous grid points and reading off the PGA for a particular q or T. Remember that q, T, L and N are related by −L i =i ∑ Ni Spectral Acceleration q = 1 − e i =1 (Poisson) and T = 1 / ΣN The Poisson distribution is stationary with time i.e. independent of time, hence the probability of earthquake occurring the year after is the same. Thus no elastic rebound theory inculcated. The hazard map allows the engineer to obtain a design PGA for a particular q or T. However, this value of PGA does not characterise the nature of strong motion and it is also of little use as an input to structural analysis except for an infinitely stiff structures. For general structures, we employ the design response spectra. (c) Uncertainties in Seismic Hazard Assessment (i) Uncertain scatter in attenuation relationship (ii) Uncertain limits of source zone and hence the value of MMAX (iii) Uncertain choice of attenuation relationship 518 Peak Ground Acceleration T Structural Engineering Analysis and Design Second Edition 5.1.1.19 Seismic Hazard Evaluation Procedure: Design Response Spectra Peak Ground Acceleration (PGA), which corresponds to the response for an infinitely stiff SDOF system or structure; Spectral Acceleration The response spectrum is a graph showing the maximum response of a range of SDOF systems, with a specific level of damping, subjected to a particular accelerogram (i.e. strong-motion). A SDOF is fully characterised by its damping level ζ and its natural period of vibration T = 2π(m/k)–½. The response spectrum is plotted by calculating the response of a series of SDOF systems (with differing T but same ζ) subjected to a particular acceleration timehistory at their base. Hence the response spectrum is a plot of relative displacement, relative velocity or absolute acceleration versus period T. Effect of sub-soil layers above bedrock rock T Period of structure should avoid plateau Effect of period of the SDOF system or structure on their response PGA is the response on an infinitely stiff SDOF system. The inclusion of the period of the SDOF system gives rise to the response spectrum. The effect of softer and less stiff (more flexible) sub-soil layer above the stiff bedrock changes the response spectrum in the following manners: (i) Amplitude of the response increases Velocity of propagation is less in soil than in bedrock. In order to maintain the energy carried by the waves, the amplitude increases and the amount depends upon the contrast in propagation velocity in the soil and the bedrock, the softer the soil, the greater the amplification. (ii) Amplitude of the spectrum increases dramatically if resonance occurs If the dominant period of the ground motion (large earthquakes tend to produce dominant long-period waves whilst smaller earthquakes produce short period waves) i.e. T1 = 4H/S coincides with the natural period of vibration of the soil layer, then resonant response can result in very high amplitudes on the spectrum at that particular period. This happened in Mexico City on the 19th of September 1985 where a large MS 8.1 earthquake caused greatest damage in the city underlain by soft lacustrine clay deposits although 400km away from the source. (iii) Duration of strong motion increases Waves can be reflected at the surface and then as they propagate downwards they can again be reflected back upwards at the rock face and in this way become trapped within the soil layer. This will have the effect of increasing the duration of the strong ground-motion. (iv) Maximum amplitude occur at higher periods for soil spectra and at lower periods for rock spectra This occurs because softer soil (less stiff, more flexible, lower frequency, higher period) tend to amplify high period waves and harder rock (more stiff, less flexible, higher frequency, lower period) tend to amplify low period waves. (v) PGA reduces The value of the PGA is also dependent upon the sub-soil conditions (stiffness) although not usually taken into account in the attenuation relationship. A soft (flexible) soil will tend to reduce the value of the PGA as low period (high frequency) waves are filtered by the soft soil. 519 Structural Engineering Analysis and Design Second Edition The earthquake magnitude M and the distance d change the response spectra in the following manner. Small nearby earthquake produce high frequency dominant waves. Large faraway earthquakes produce low frequency dominant waves. Spectral Acceleration The seismic hazard assessment procedure by the method of design response spectrum involves either: (a) PGA determination from hazard map and spectral shape fixation from codes of practice PGA = corresponds to the response for an infinitely stiff SDOF system or structure = obtained from the hazard map = function of (M, distance d, return period T and probability of exceedance q) although also dependent upon the soil stiffness Spectral Shape = corresponds to the response of a variety SDOF system or structure with different stiffnesses (or periods) = function of (SDOF or structure period, soil stiffness) although also a function of the earthquake magnitude in that the peak amplitude varies with M M7 M6 T M5 (b) Response spectral ordinates The response spectrum can also be obtained from equations predicting the response spectral ordinates. Such equations are derived in exactly the same way as attenuation relationships for PGA for a number of different response periods. Response spectral ordinate equation = function of (M, distance d, SDOF period T, soil stiffness) The response spectra by including the PGA, the spectral shape and its amplitude, accounts for M, d, the structural periods T and soil stiffness. The response spectrum falls short in the sense that the duration of the earthquake not accounted for. Long duration earthquakes are obviously more damaging. Duration is a function of M, the larger the M, the longer the duration. The larger the earthquake the longer the duration, the longer the period of the waves and the larger the spectral amplitudes. 520 Structural Engineering Analysis and Design Second Edition 5.1.2 Effect of Local Soil Conditions on the Seismic Hazard 5.1.2.1 Elastic Soil Properties The elastic properties of soil are defined by the following 3 parameters: (a) the mass density, ρ (b) the elastic moduli (i) the shear wave velocity S or VS is measured S or VS obtained from explosion tests, or S or VS = 85 N600.17 (Dm)0.2 (Seed 1986 empirical using SPT and CPT tests) (ii) Shear modulus G is computed from the shear wave velocity S µ G = ρ ρ S= (iii) (iv) Poisson’s ratio ν known Young’s Modulus E computed G= (v) Lame’s constant λ computed; Note the other Lame’s constant µ λ= (vi) E 2(1 + ν) Eν (1 + ν )(1 − 2ν) µ=G compression wave velocity C is computed C= λ + 2µ ρ (c) the damping σ γ ∆W = area under loop = energy lost in one loading-unloadingreloading cycle W = area under the triangle 1 ∆W Damping coefficient, ζ = 4π W Logarithmic decrement, δ = 2πζ 521 Structural Engineering Analysis and Design Second Edition 5.1.2.2 Dynamic Response of Soil The dynamic response of soil depends upon: (a) whether the loading is small strain loading or large strain loading Earthquake loading may either be small strain or large strain. The shear modulus G and damping ζ of the soil depends on the strain level, hence non-linear behaviour. The shear modulus is represented by the secant modulus at any given strain. G ζ γ γ Small Strain Loading Large Strain Loading High G, low ζ Low G, high ζ Soil can be modeled as viscoelastic material Soil cannot be modeled as viscoelastic material as it is non-linear. Ground motion controlled by limit strength of soil. Hence the critical acceleration i.e. the limit acceleration the soil can transmit is used. Field measurements of shear wave velocities In general, G at any strain level can be related to generally give those at very low strain levels. This GMAX although the relationship differs from soil to yields the maximum shear modulus GMAX. soil. (b) whether the loading is monotonic or cyclic Dry soils or Undrained saturated soils drained saturated soils No change in Collapsible soil Non-collapsible soil strength with τ cycles. τ Behaviour under cyclic γ γ loading same as that under Pore pressures rise continuously with cycles Pore pressures rise then tend to decrease monotonic Strength peaks and then reaches residual Strength increases loading. Strain softening material Strain hardening material (c) (d) (e) (f) Stress (in the form of liquefaction) and Strain is the criteria for failure, whilst stress strain is the criteria for failure failure (in the form of liquefaction) unlikely Loose cohesionless sands Dense sands Normally consolidated clays Overconsolidated clays Note that the damping increases with cyclic loading. the frequency of the loading the speed of loading i.e. the rate of strain Sand: the strain-rate has little effect on the strength Clay: the strain-rate has considerable effect on the strength whether sliding occurs or not If sliding occurs, strain is no longer applicable. the stress path The undrained strength and the pore water pressures are stress path dependent and therefore limit strength of soil depend on how the failure state is arrived at. Since a soil element is subjected to 3 normal stresses and 3 shear stresses, the limit strength will depend on how each component is varied in the field during an earthquake. 522 Structural Engineering Analysis and Design Second Edition 5.1.2.3 Liquefaction Liquefaction means failure due to rise on pore water pressures, and is not necessarily associated with a complete loss of strength. Hence, liquefaction is denoted by either of the following mechanisms: (a) ZERO EFFECTIVE STRESS IN LOOSE SOILS: Zero effective stress (and hence zero shear strength, i.e. complete loss of strength) occurs due to rise in pore water pressures; this occurs when the structure of loose saturated cohesionless soil collapses due to vibration and cyclic loading. When shear stress is applied under no volume change condition, some grains may lose contact with neighbouring grains, and therefore part of the load is taken up by the water. Thus excess pore water pressure is generated. On unloading, these grains do not go back to its original position and therefore, the excess pore water pressure remains. On further loading or reverse loading, more grains lose contact and more excess pore pressure is generated. Finally, after a number of cycles, if there is the possibility for all grains to separate from each other, then the entire load before cycling is taken up by the water and true liquefaction occurs. For this state to occur, the soil must be in very loose state at the beginning. After liquefaction, the liquefied soil will end up in a denser state in time through the dissipation of the excess pore pressure. In such a soil, collapse of the soil may take place even in static loading and shows very low residual strength. (b) CYCLIC MOBILITY IN MEDIUM DENSE TO DENSE SOILS: Cyclic mobility i.e. the accumulation of large strains (or displacement along a shear surface) during cyclic loading is caused by the reduction of effective strength as a result of accumulation of pore water pressure. In defining cyclic mobility, there is thus no association with a complete loss of strength. However, the accumulation of strain may become very large and the soil may be considered as failed although the strength of the soil does not decrease as a whole even after failure. CYCLIC MOBILITY IN MEDIUM DENSE TO DENSE SOILS (Non-Collapsible) ZERO EFFECTIVE STRESS IN LOOSE SOILS (Collapsible) Loose soils Medium dense to dense soils Low residual strength Strength of soil does not decrease as a whole Low strains Large strains signifying failure The cause of liquefaction in the field is the collapse of loose saturated cohesionless soils due to either: (a) cyclic loading, or (b) static loading (quick sand conditions) Manifestations of the liquefaction phenomenon include: (a) Bearing capacity failure in level ground causing tilting and sinking of structures (b) Ground oscillation on very mild slopes, no lateral spreading but ground breaks into blocks which oscillate causing the opening and closing of fissures (c) Lateral spreading of mild slopes with a cut or free slope due to the liquefaction of sub-surface deposits; ground breaks up causing large fissures and the ground generally moves slowly down the slope (d) Flow failure of steep slopes due to liquefaction of the slope causing landslides, common in mine tailings (e) Sand boils which are evidence of high pore water pressures at some depth due to liquefaction (f) Rise of buried structures such as water tanks and timber piles which are lighter than the liquefied deposits (g) General ground settlement occurring due to the densification of deposits after liquefaction (h) Failure of quay walls (retaining walls) due to the increase of pressure on the wall as a result of liquefaction 5.1.2.4 Residual Strength of Liquefied Soils The residual strength of liquefied soil is an important parameter for estimating the stability of liquefied soils. The residual strength depends mainly on the void ratio but several other factors are noted, namely the initial confining pressure, the soil fabric, the fines content and the particle size and shape. The strength increases with increasing overconsolidation ratio. Increasing fines content decreases the steady strength at the same relative density. 523 Structural Engineering Analysis and Design Second Edition 5.1.2.5 Assessment of Liquefaction Potential The liquefaction potential of a site depends on: (a) the size of the earthquake measured by MS or MW, preferably the latter (b) the distance of the earthquake from the site (c) the CRR values in terms of N160 or qc1N or VS1 of the deposits (d) the position of the water table with respect to the deposits Liquefaction is most likely in loose saturated cohesionless sands. Gravelly soils being more permeable are unlikely to liquefy, although liquefaction of sandy gravel has occurred in the Kobe earthquake. But generally, the liquefaction resistance of sand-gravel composites increases considerably with increasing gravel content. Most clayey soils on the other hand are not vulnerable to liquefaction. However, laboratory studies indicate some loss of strength during cyclic loading and cyclic mobility may be significant. Increased plasticity generally increases the cyclic strength. The assessment of the liquefaction potential is as follows: aMAX.g h τ γ liquefiable soil layer (a) Cyclic stress ratio CSR The CSR depends on the shear stress imposed by the earthquake as a function of the initial effective overburden pressure. This therefore depends primarily on the magnitude and distance of the earthquake, the depth of the liquefiable soil, the depth of the water table and the characteristics of the soil layer. CSR = τ / σ’ = 0.65 (aMAX) (γh/σ’) rd where h = depth to point of measurement or liquefiable soil rd = rigidity of soil to include the effect of more flexible soil at depth, hence lower shear stresses = generally, rd varies from 1 at the surface to 0.9 at 10m depth = a function of the depth to the liquefiable layer, for instance 1-0.00765z (Liao & Whitman 1986) γh = total overburden pressure at the level of the liquefiable layer σ’ = effective overburden pressure at the level of the liquefiable layer aMAX = peak ground acceleration at site from an attenuation relationship based on a maximum MW log(aMAX) = –1.02 + 0.249MWMAX – log(r) – 0.0025r where r2 = Rf2+53.3 (Joyner & Boore 1981) note that τ = mass/area x acceleration = γh/g x apeak note that γh/σ’ takes the position of the water table into account note that 0.65 of aMAX represents 95% energy of the record note that as with most attenuation relationships, aMAX is the numerical fraction of g (b) Cyclic resistance ratio CRR The CRR depends on the quality of the soil and the depth of the liquefiable layer. This is defined as the cyclic stress required to cause liquefaction in a given number of cycles expressed as a fraction of the initial effective confining pressure. CRR is the required CSR for liquefaction. The CRR values are usually determined for liquefaction at 15 cycles of loading representing a 7.5 magnitude earthquake. Since the number of cycles is a function of the duration of the earthquake, which in turn depends on the magnitude, CRR is dependent on the magnitude of the earthquake as well. The factors effecting the CRR are void ratio and relative density, overconsolidation ratio, fines content and plasticity of fines. CRR can be determined from shear box and triaxial tests, but field measurements are preferable. CRR can be determined in the field by either one of the following methods: (i) CRR from SPT (standard penetration test) blow count N procedure Normalised SPT value to depth and energy efficiency N160 = N.CN E / 60 where N = measured blow count 524 Structural Engineering Analysis and Design Second Edition CN = depth normalisation factor = (100/σ’)0.5 or 0.77log10(2145/σ’) σ’ = effective stress at the point of measurement i.e. at the depth of the liquefiable soil (kPa) E = energy efficiency of the SPT (%) CRR = function of (N160, MW, fines content) obtained through field observation of liquefaction (ii) CRR from CPT (cone penetration test) tip resistance qc procedure CPT is better than SPT in the sense that it provides a continuous reading unlike SPT which are taken at intervals. Also, repeatability with SPT tests is poor. Normalised CPT value qc1N = qc (100 / σ’)0.5 / 100 where qc = measured tip resistance (kPa) σ’ = effective stress at the point of measurement i.e. at the depth of the liquefiable soil (kPa) CRR = function of (qc1N, MW, fines content) (iii) Shear wave velocity procedure The use of S or VS is advantageous because this can be measured easily with accuracy in soils in which SPT and CPT are difficult to perform. The disadvantage is that it is measured in situ with very small strains. Moreover, seismic testing is done without extracting samples and as such, difficult to identify non-liquefiable low velocity layers (soft clay rich soils) or liquefiable high velocity layers (weakly cemented soils). However, shear wave velocity measurements along with bore-hole data becomes very usable. Normalised shear wave velocity VS1 = VS (100 / σ’)0.25 where VS = measured shear wave velocity σ’ = effective stress at the point of measurement i.e. at the depth of the liquefiable soil (kPa) CRR = function of (VS1, MW, fines content) (c) Factor of safety against liquefaction FL = CRR / CSR Note that if FL > 1.0, then no liquefaction. CSR Liquefaction Base curve for MW = 7.5 and a certain % of fines Inputs: CSR and N160 or qc1N or VS1 No Output: whether liquefaction occurs or not Liquefaction N160 or qc1N or VS1 Note that, for the same N value, higher percentage of fines shows higher CRR. There is good agreement between the SPT and CPT procedures. Beyond N160 > 30 or qc1N > 160, according to the NCEER (1997), liquefaction is very unlikely to occur. The base curves are plotted for a MW of 7.5. For other magnitudes, scaling factors (MSF) are proposed which multiply the CRR base curves. The reason that large magnitude earthquakes may liquefy sites at large distances even though the corresponding acceleration is small is due to the longer duration and therefore to the larger number of cycles. Liquefaction can be achieved by smaller number of cycles with large stress amplitudes and by larger number of cycles with smaller stress amplitudes. 5.1.2.6 Post-Seismic Failure due to Liquefaction The consolidation of a liquefiable soil at a depth underneath a competent soil with time may increase the pore pressures in the top layer causing bearing capacity failure some time after the earthquake. The upward flow may even cause piping failure. The delay depends on the relative consolidation and swelling properties of the two layers. 525 Structural Engineering Analysis and Design Second Edition 5.1.2.7 (a) (b) (c) (d) (e) Methods of Improving Liquefiable Soils Remove and replace unsatisfactory material (i.e. loose saturated cohesionless sands) Densify the loose deposits Improve material by mixing additives Grouting or chemical stabilisation Draining solutions 5.1.2.8 Effect of Soil Layer on Ground Response The effect of local soil layer is as follows: (a) Impedance (or radiation) effect, hence increase in amplitude of strong motion (b) Increase in duration of strong motion as energy becomes trapped within soil layer (c) Resonance effect, hence a great increase in amplitude of strong motion We consider vertically propagating polarised shear wave in energy transfer because: (a) due to the continuously decreasing stiffness of the soil or rock material, the wave front appears to travel vertically; an elastic wave propagating to a less stiff material (such as from stiffer rock to soil) will begin to propagate slower, since VS = (G/ρ)0.5 i.e. VS ∝ G0.5 ∝ E0.5 and ρrock ~ ρsoil. A wave propagating slower will tend to move towards the normal to the interface between the 2 mediums. (b) at a reasonable distance form the focus, these spherically propagating waves may be considered as plane propagating waves in a narrow wave front (c) the energy carried by the shear waves is more important than that carried by the compression waves, these two waves being the only two emitted from the focus 5.1.2.9 Motion of Shear Waves in Elastic Media The motion of shear waves in elastic an elastic medium is given by the equation of motion 2 ∂ 2u ∂ 2u  2 ∂ u s = + η   2 ∂t 2 ∂y 2   ∂y for which the solution is u = Ae -λΩs/S e iΩ ( y / S− t ) where s = distance travelled within damped soil (m) y = vertical displacement (m) t = time (s) S = shear wave velocity (ms -1 ) Ω = circular frequency of the wave (rad/s) = 2πf = 2π / T λ = ηΩ/2 (damping as a fraction of critical) Ae -λΩs/S = decaying amplitude term suggesting higher frequency waves decay faster e iΩ ( y / S− t ) = harmonic term, i.e. same response shown periodically 526 Structural Engineering Analysis and Design Second Edition 5.1.2.10 Impedance (or Radiation) Effect The impedance effect occurs because of the contrast of properties at the rock-soil interface. A B H ROCK Sr, ρr SOIL Ss, ρs Arefracted Ain Areflected (a) Impedance relationships A in = Amplitude of incoming wave A refracted = Sρ 2 1− r A in & A reflected = A in where r = s s 1+ r 1+ r Sr ρ r (b) Amplitude of concern, Aboundary The wave motion at the boundary is the same whether one looks at it from the first or the second medium. A boundary = A refracted = A in + A reflection For r = 0 : free boundary with A boundary = 2A in r < 1 : rock to soil with A refracted > A in r > 1 : soil to rock with A refracted < A in r = 1 : no boundary with A refracted = A in (c) Typical values S s = 300 ms −1 , S r = 3000ms −1 , ρ s ≈ ρ r , ∴ r = 0.1, A refracted = 1.82A in & A reflected = 0.82A in Notice that the soil has amplified the motion of the waves as they were impeded. (d) Computation procedure for first half-cycle of strong-motion at site ASOIL@B INPUT : A ROCK@A is an A boundary obtained from the attenuation relationship from a seismic hazard analysis METHOD : A in = Amplitude of incoming wave = A ROCK@A / 2 as A boundary = 2A in : A refracted = Sρ 2 A in where r = s s 1+ r Sr ρ r OUTPUT : A SOIL@B = 2A refracted e -λΩs/S as A boundary = 2A in On the soil spectra, the effect of impedance is as follows: (a) Amplitude of the response increases The effect of impedance is to increase the amplitude of the strong motion response. Velocity of propagation is less in soil than in bedrock. In order to maintain the energy carried by the waves, the amplitude increases and the amount depends upon the contrast in propagation velocity in the soil and the bedrock, the softer the soil, the greater the amplification. The energy flux of the incident wave is shared between the refracted and reflected waves. 527 Structural Engineering Analysis and Design Second Edition 5.1.2.11 Increase in Duration of Strong Motion Waves can be reflected at the surface and then as they propagate downwards they can again be reflected back upwards at the rock face and in this way become trapped within the soil layer. This will have the effect of increasing the duration of the strong ground-motion. Computation of strong motion response with time: (a) Establish the input Duration of earthquake wave D (s) Fundamental period of earthquake wave T (s) Damping of soil ζ Relative property of soil-rock r = Ssρs / Srρr Relative property of rock-soil r = Srρr / Ssρs (b) Establish the changes in amplitude A B A1 A1 A3 A3 A5 A5 H ROCK Sr, ρr Arefracted A2 A4 SOIL Ss, ρs Ain (i) Ain = AROCK / 2 (ii) Arefracted = 2Ain/(1+r) @ t=0 for duration D (iii) A1 = Arefracted e-ζΩs/S @ t=H/S for duration D (iv) A2 = (1-r)/(1+r) A1 e-ζΩs/S @ t=2H/S for duration D (v) A3 = A2 e-ζΩs/S @ t=3H/S for duration D (vi) A4 = (1-r)/(1+r) A3 e-ζΩs/S @ t=4H/S for duration D (vii) etc…Ainfinity until negligible amplitudes (c) Superpose waves at the top of soil layer for an estimate of a measured record A sinusoidal wave of 2A1 starting @ t=H/S for duration D A sinusoidal wave of -2A3 starting @ t=3H/S for duration D A sinusoidal wave of 2A5 starting @ t=5H/S for duration D A sinusoidal wave of -2A7 starting @ t=7H/S for duration D etc… All the individual waves have the same period and duration. Their amplitudes are doubled because of the free surface boundary. Every other wave has an opposite initial amplitude because when the waves get reflected at the bottom of the soil against the rock, there is a 180 degree phase change. These superposed waves will result in a summation wave that is increasing to a peak then decaying gradually. 2A1 wave -2A3 wave (d) Check if resonance is likely to occur Evidently, if the period of the initial earthquake incident wave is 4H/S, this would correspond to one loop cycle and resonance would occur. Also, resonance can occur if the earthquake wave period corresponds to the higher mode periods of the soil. In summary, if the earthquake period is any of the following, then resonance can occur. Mode periods of the soil Tn = T1 / (2n-1), where n = 1,2,3,4… and T1 = fundamental mode period On the soil spectra, the duration of strong ground motion is increased. 528 Structural Engineering Analysis and Design Second Edition 5.1.2.12 Resonance Effect The fundamental mode of period of the soil layer, T = 4H/Ss. Hence, the period along with the damping coefficient ζ give the layer characteristics. Thus for the same stiffness of material, the deeper the layer, the longer the period. Alternatively, for the same depth of layer, the weaker the layer, the longer the period. Earthquakes that can affect an engineering site: (a) Small earthquakes nearby (near source) Bedrock motion is rich in high frequency waves (low period) Shallow H and stiff (high S) subsoil (low period) will magnify the bedrock motion in resonance Deep H and weak (low S) subsoil (high period) will not magnify the bedrock motion in resonance (b) Large earthquakes afar (far source) Bedrock motion is rich in low frequency waves (high period) because high frequency waves decay fast Shallow H and stiff (high S) subsoil (low period) will not magnify the bedrock motion in resonance Deep H and weak (low S) subsoil (high period) will magnify the bedrock motion in resonance On the soil spectra, the effect of resonance is as follows: (a) Maximum amplitude occur at higher periods for soil spectra and at lower periods for rock spectra This occurs because softer soil (less stiff, more flexible, lower frequency, higher period) tend to amplify high period waves and harder rock (more stiff, less flexible, higher frequency, lower period) tend to amplify low period waves. (b) PGA reduces The value of the PGA is also dependent upon the sub-soil conditions (stiffness) although not usually taken into account in the attenuation relationship. A soft (flexible) soil will tend to reduce the value of the PGA as low period (high frequency) waves are filtered by the soft soil. (c) Amplitude of the spectrum increases dramatically if resonance occurs If the dominant period of the ground motion (large earthquakes tend to produce dominant long-period waves whilst smaller earthquakes produce short period waves) coincides with the natural period of vibration of the soil layer (i.e. 4H/Ss), then resonant response can result in very high amplitudes on the spectrum at that particular period. This happened in Mexico City on the 19th of September 1985 where a large MS 8.1 earthquake caused greatest damage in the city underlain by soft lacustrine clay deposits although 400km away from the source. Near Source Far Source Response Spectra due to Near Source and Far Source Events 529 Structural Engineering Analysis and Design Second Edition 5.1.2.13 Methods of Evaluating Layer Response Three methods can be used, namely: (a) The travelling wave method This has been described in the Increase in Duration of Strong Motion section (b) The Square Root of Sum of Squares (SRSS) method Characteristics: Infinitely stiff rock base Provides steady state and transient state solutions Only good to find maximum acceleration AMAX, i.e. no time history response Damping coefficient refers to the modal damping If we treat soil as an elastic material, then a column of soil over the rock (assumed rigid since Sr >> Ss) behaves like any other structure which has natural modes and mode shapes. The solution to such a problem is & u&( y, t ) = ∞ ∑ Φ ( y, n ) I ( t , n ) n =1 Φ ( y, n ) = mode shapes depending on geometry and boundary conditions I(t, n) = response of SDOF systems of mode frequencies subjected to the applied load Thus, a soil layer (or any elastic structure resting on a rigid base) is equivalent to a series of SDOF pendulums (characterised by their ω and λ) standing on a single rigid base. The total response of the soil layer is obtained by combining all the responses of each SDOF system. Peak acceleration, & u&( y) MAX = ~4 ∑Φ 2 ( y, n )S a2 (n ) n =1 Sa is the equivalent acceleration spectrum values of the acceleration record. Note only 4 modes are used in the SRSS method. Note also that y=0 at the free surface and is measure positive downward. INPUT: soil damping ζ, forcing frequency Ω (rad/s), soil layer H (m), soil shear velocity Ss (ms-1) Mode Frequency of system, Period of system n Sa = function (ζ, Ω, ω) φ2 Sa2 φ2 x Sa2 T = 4H / [(2n-1)S] shapes, φ ω = 2π/T 1 . . 4 AMAX = SQRT(Σn=1-4 φ2 x Sa2) (c) The SHAKE method Characteristics: Base rock is considered flexible, hence radiation damping i.e. waves that travel into the rock from the soil, is taken into account Provides only steady state solution Gives time history response Different layers can have different damping coefficients In this technique, a single harmonic component of the wave can be transferred from any known point to any other desired point by the use of a complex transfer function. By using Fourier Series of the known motion, each component of the series can be transferred to the desired point and by using the superposition technique, these component waves can be recombined to produce the time history of the motion at the desired point. Hence, the SHAKE method is summarised as follows: I. input is the ground motion f(t) II. f(t) is decomposed into multiple frequency Ω waves each having an amplitude A and phase θ III. for each component wave Ω, the transfer function of amplitude T and of phase φ is computed output wave component amplitude is TA and phase is θ + φ next component wave IV. the output wave components are superimposed for a time history response 530 Structural Engineering Analysis and Design Second Edition 5.1.2.14 Critical Acceleration Small Strain Loading Large Strain Loading Soil cannot be modeled as viscoelastic material as it is non-linear. Ground motion controlled by limit strength of soil. Hence the critical acceleration i.e. the limit acceleration the soil can transmit is used. Soil can be modeled as viscoelastic material A B h weak layer SOIL ROCK (a) Limit undrained strength of weak layer, cu ∆u = B[∆σ 3 + A (∆σ1 − ∆σ 3 )] (Skempton' s) c' cos φ'+ σ' [K 0 + A (1 − K 0 )]sin φ' 1 - (1 - 2A)sinφ' Note that the change of pore water pressure ∆u is dependent upon the change of principal stresses due to an earthquake. For saturated soils, B = 1. Under cyclic loading the pore pressure parameter A changes with cycles. The effect of rotation of the principal stresses is not taken into account. The undrained strength depends upon the change of pore water pressures. Hence, both ∆u and cu are dependent upon the number of cycles. (b) Applied stress at weak layer, τ Applied stress, τ = force/area x acceleration = m/A x a = ρVa/A = ρhAa/A = ρha = γha/g (i.e. total stress / g x acceleration) = γhkmg/g as a = kmg = γhkm (c) Critical acceleration When τ = cu then the acceleration is critical For c’ = 0, τ = cu [K + A(1 − K 0 )]sin φ' α= 0 γhkc = σ1’α 1 - (1 - 2A)sinφ' kc = σ1’α/γh = α σ1’/σ1 For c’=0, and say φ’=30°, K0=0.6, sinφ’=0.5, A=0.4 and with water table at ground level, kc = 0.42γ’/γ = 0.2. This means that, the weak soil layer will fail if a=0.2g. (d) Consequences If the elastic response predicted a magnified acceleration at B of say 0.5g from an incoming acceleration of 0.2g at A, this non-linear critical acceleration analysis will tell us that in actual fact the response at B would be truncated to 0.2g. However, the upper part of the soil will behave like a sliding block trying to move over the sliding surface and we may see ground cracks on the surface. This sliding block displacement is predicted by log(umax)=f(kc/km) where kcg = critical acceleration kmg = maximum elastic acceleration such as log(4umax/CkmgT2)=1.07-3.83kc/km (Sarma 1988); Hence, (i) if elastic response km < critical kc, km applies and no sliding block displacement (ii) if elastic response km > critical kc, kc applies and there is a sliding block displacement. Undrained strength, c u = 531 Structural Engineering Analysis and Design Second Edition Accn 5.1.2.15 Effect of Local Soil Conditions on Seismic Hazard Design Procedure Summary The objectives of the analysis are: (a) to provide a soil surface acceleration response taking into account the properties of the soil layers overlying the rock. The peak ground acceleration of the free-field rock is 0.6g from the previous seismic hazard assessment of Section 5.1.1.18. (b) to assess the liquefaction hazard of the site 5.1.2.15.1 Soil Surface Acceleration Response (a) Design Rock PGA from the Seismic Hazard Analysis (b) Design Free-Field Rock Acceleration Time History Plot of acceleration (g) with respect to time as measured on the free-field rock scaled to the design PGA from the hazard analysis of (a). (c) Acceleration Spectrum of the Free-Field Record Plot of spectral acceleration (maximum acceleration) with respect to the period of the structure. This response spectrum shows the maximum response (in terms of acceleration) of a range of single degree of freedom systems with a specified level of damping subjected to the above free field rock acceleration time series. The PGA is the intersection at the vertical axis and its value is the maximum observed on the acceleration time series of (b), i.e. the response of an infinitely stiff structure. In short: PGA Time (s) Spectral Accn Acceleration time series of an infinitely stiff structure PGA (Ti , Aipeak) Accn Apeak Ti Period of Structure Time (s) Acceleration time series of an finitely stiff structure of period Ti Alternatively, the rock acceleration spectrum can be obtained from the fixation of a spectrum shape (from the design codes) to the design rock PGA of (a). Thirdly, the rock acceleration spectrum can also be obtained from spectral ordinates. (d) Fourier Spectrum of the Rock Record Plot of modulus with respect to frequency (or period) of the earthquake wave derived from the time series of (b). The Fourier spectrum is a mathematical representation of the infinite wave harmonics that make up the earthquake wave record time series of (b). That is to say, the earthquake record can be broken up into an infinite number of waves defined by an amplitude and frequency. The Fourier Spectrum of the rock record is thus the mathematical representation of the earthquake wave harmonics prior to modification due to the soil layers. Two graphs define the Fourier spectrum, namely the modulus versus frequency graph and the phase versus frequency graph. The frequency at which the maximum modulus occurs is the dominant frequency of the earthquake wave time series prior to modification by the soil layers. Fourier Spectrum = ∑a ne i ( ωn t − φ ) (e) Shear Wave Velocity Profile Plot of shear wave velocity with respect to depth. Shear wave velocity, VS (m/s) = 85 N600.17 (Dm)0.2 i.e. based on the SPT. However it is best to carry out proper seismic blast tests. (f) Transfer Function Plot of modulus with respect to frequency of the waves derived from the shear wave velocity profile of (e). 532 Structural Engineering Analysis and Design Second Edition (g) Fourier Spectrum of the Soil Surface Plot of modulus with respect to frequency (or period) of the earthquake wave. The Fourier Spectrum of the soil surface is the mathematical representation of the earthquake wave harmonics after the modification due to the soil layers. These are obtained by multiplying the Fourier spectrum of the rock record by the transfer functions. The dominant frequency of the earthquake waves are usually lower in the soil modified Fourier spectrum compared with the rock Fourier spectrum. This is expected as the more flexible (high natural circular period) soil layers tend to lower the frequency (or increase the period) of the earthquake waves. (h) Design Soil Surface Acceleration Time History Plot of acceleration (g) with respect to time obtained from the Fourier spectrum of the soil surface of (g). (i) Acceleration Spectrum at the Soil Surface Plot of spectral acceleration (maximum acceleration) with respect to the period of the structure. This response spectrum shows the maximum response (in terms of acceleration) of a range of single degree of freedom systems with a specified level of damping subjected to the above soil surface acceleration time series of (h). The PGA is the intersection at the vertical axis and its value is the maximum observed on the acceleration time series of (h), i.e. the response of an infinitely stiff structure. (j) Maximum Shear Stress Profile & Shear Strength Profile The maximum shear stress τapplied profile (plot of shear stress with respect to depth) is obtained from the accelerations at each level of the profile. The maximum shear strength τcapacity profile is obtained from cu c' cos φ'+ σ' [K 0 + A (1 − K 0 )]sin φ' τ applied = c u = 1 - (1 - 2A)sinφ' Damping % Shear Modulus, G Wherever τapplied > τcapacity, the critical acceleration has been exceeded. (k) Applied Acceleration Profile & Critical Acceleration Profile Applied acceleration km = τapplied / γh and critical acceleration kc = τcapacity / γh. (l) Soil Surface Design Acceleration Define the minimum critical acceleration as the smallest critical acceleration within the soil profile considered. Hence, the soil surface design acceleration is the smaller of: (a) the minimum critical acceleration kcmin, and (b) the elastic response at the soil surface, which is given for different periods (of the SDOF structures), in the response spectrum of (i) (m) Effect of Large Strains on Shear Velocity The shear modulus, G decreases with strain. Since shear wave velocity, S is proportional to G0.5, S will also decrease with large strains. When there is large strain, soil particles are not as tightly packed, thus the shear wave cannot travel as quickly. The reduction in shear velocity will cause a slight reduction in the dominant frequency of the earthquake waves because of the increase flexibility of the soil layers. However, the consequences of this are minimal. Strain % (m) Sliding Block Displacement Sliding block displacement occurs whenever km > kc This sliding block displacement is predicted by log(umax)=f(kc/km) where kcg = critical acceleration kmg = maximum elastic acceleration such as log(4umax/CkmgT2)=1.07-3.83kc/km (Sarma 1988); 5.1.2.15.2 Liquefaction Hazard Analysis Cyclic Stress Ratio CSR Shear Soil Unit Layer Depth Stress, τ rigidity, Weight No (m) rd (kN/m3) = kmγh σ' Cyclic Resistance Ratio CRR CSR = 0.65τ rd / σ' N60 The liquefaction hazard is ascertained from graphs of CSR versus N160. 533 Depth normalisatio n factor, CN = (100/σ')0.5 N160 = CNN60 Liquefaction if CSR>CRR Structural Engineering Analysis and Design Second Edition 534 Structural Engineering Analysis and Design Second Edition 535 Structural Engineering Analysis and Design Second Edition 536 Structural Engineering Analysis and Design Second Edition 537 Structural Engineering Analysis and Design Second Edition 538 Structural Engineering Analysis and Design Second Edition 539 Structural Engineering Analysis and Design Second Edition 540 Structural Engineering Analysis and Design Second Edition 541 Structural Engineering Analysis and Design Second Edition 5.1.3 5.1.3.1 Conceptual Structural Design for RC Structures in Seismic Regions 8 Plan Layout Rectangular plan shapes are preferable to winged, T, L or U shapes. Winged structures and structures with reentrant corners suffer from non-uniform ductility demand distribution. Torsional effects are evident when the centre of mass (centre of application of inertial loads) and the centre of stiffness are offset. A couple which increases the shear forces on the columns then occur. Also, extended buildings in plan are more susceptible to incoherent earthquake motion, being founded on different foundation material. Aspect ratio 1 to 3 at most, otherwise use seismic joints. Building extended in plan will be subjected to asynchronous motion especially when founded on soft ground and should be avoided. Otherwise, seismic joints should be used to separate parts of the building along a vertical plane. In which case, the minimum separation between two adjacent parts should be calculated to ensure that no pounding occurs. Re-entrant corners resulting from T, L or U plan shapes attract high demands and should be avoided. The plan stiffness and strength distribution should be carefully checked and should be close to the centre of mass to avoid undue damaging effects of rotational response. 5.1.3.2 Elevation The aspect ratio of the building in elevation affects the overturning moment exerted on the foundations. Low height to width aspect ratio is desirable. Also, very slender structures suffer from higher mode contributions, thus necessitating the use of more elaborate seismic force calculations. Differences of more than 20-25% in mass or stiffness between consecutive floors should be avoided. Mass concentrations should be avoided. Stiffness discontinuity (soft storeys) should be avoided i.e. higher storeys or a storey without infill panels whilst all other storey has should be avoided. Bridges between structures should be on rollers to minimize interaction. Irregularities in elevation exert concentrated ductility demand such as when a multibay tall building is taller in just one of the bays instead of all the bays. The stiffness difference between two consecutive storeys should not exceed 25%. This not only implies that column sizes should not change drastically but also means that set-backs should be kept to a minimum. The total mass per floor should also conform to the same limits of variation. No planted columns should be allowed and no interruption of shear walls, where provided, should be permitted. Where column size and reinforcement is reduced with height, extreme care should be exercised at the location of such a change to ensure a uniform distribution of ductility demand. The aspect ratio in elevation should not be excessive; a height to width ratio of about 5:1 is reasonable. Whenever possible, the foundation level should be kept constant to avoid excessive demand being imposed on the shorter columns responding mainly in shear. 5.1.3.3 Beam and Column Axes All beams and columns should have the same axes with no offset between adjacent members. Avoid columns supported on beams as imposed local demand in shear and torsion is considerable. Avoid partial infill panels as these create short columns susceptible to failure by shear cracking, just like link beams. 8 ELNASHAI, Earthquake Engineering Seismic Analysis Lectures. Imperial College of Science Technology and Medicine, London, 2001. 542 Structural Engineering Analysis and Design Second Edition 5.1.3.4 Foundation Design Forces on footings and bearing capacity underneath footings should be calculated from the worst case scenario of dead and live load combined with maximum over-turning moment and vertical earthquake component. For simplicity, the base shear may be applied at a point 2/3 of the height of the building from the base for the calculation of over-turning moment. When there is no raft (mat) foundations, footings should be tied by RC beams with minimum reinforcement ratios. The point of connection of the tie beams should not be higher than the soffit of the footing, since this creates a short member which may be susceptible to shear failure. 5.1.3.5 Columns Plastic hinges are allowed at the base of ground floor columns, but not at their tops. Transverse reinforcement should be provided in the lower ¼ of the column height at a minimum spacing. This may be increased in the middle region, but should be decreased again at the top of the column. Stirrups are all to have bending angle of 135 degrees or more, since 90 degrees stirrups are proven to be ineffective. Alternatively, the EC8 detailing requirements should be followed. Strictly, no hinging columns above the ground floor should be allowed. In practice though, observations have indicated that limited hinging in a limited number of columns within a storey may be tolerated provided that a storey sway mechanism is completely avoided. The top and bottom ¼ column heights should be adequately confined by closed stirrups. These should be bent as above. 5.1.3.6 Member Capacity at Connections To realize the weak beam and strong column response mode, beam capacity should be about 20%-25% lower than the capacity of the column, taking into account a conservative estimate of the effective width of the slab. This is one of the most important aspects of capacity design for seismic action. In this calculation, the actual areas of steel used should be accounted for, and not the design value. Also, this calculation should not include any material partial safety factors. Finally, for conservatism, the beam steel yield should be increased by about 10% to account for strain hardening. In one of each four columns in a storey, this condition may be relaxed. Also, this condition does not apply to top floor columns, where the rule can be relaxed. The resistance mechanism in connections should be checked for the loading case with minimum gravity loads and maximum overturning, to ascertain that there is sufficient shear resistance even when the concrete contribution is at a minimum. The closely spaced stirrups used for column head and base should be continued into the beam-column connection. Also, beam reinforcement should be carefully anchored, especially in exterior connections. If the development length is sufficient, a column stub should be used to anchor the beam reinforcement. 5.1.3.7 Floor Slabs Large openings should be avoided since the slabs are responsible for distributing the floor shear force amongst columns and reductions in their stiffness is not conducive to favourable seismic performance due to loss of diaphragm action. 5.1.3.8 Infill Panels Masonry or block concrete infill panels should be protected against dislocation and shedding. Where provided, they should not be interrupted as to form short columns in adjacent members. 543 Structural Engineering Analysis and Design Second Edition 5.1.3.9 Building Separation For adjacent buildings, a minimum separation is essential. This may be calculated according to a seismic code. A conservative approach is to calculate the elastic displacement under the design event and multiply it by the behaviour factor used in design. The resulting displacement should not lead to pounding at any level. If the structure in the vicinity is of drastically different dynamic characteristics, then its displacement, calculated as above, should be added to that of the building under consideration to arrive at the required gap width. For structures of largely similar characteristics founded on similar soils, some proportion of the sum of the two displacements may be used. There is no global agreement on this proportion. 5.1.3.10 Architectural Elements These are part of the structure and should be treated as such. They should either be designed to resist the forces and especially the deformations imposed on them, or separated from the lateral load resisting system. The consequence of their damage and shedding should be verified with regard to life safety and interruption of use. 5.1.3.11 General Robustness All parts of the structure should be tied to ensure a monolithic response under transverse vibrations. This includes all structural and non-structural components in the two orthogonal directions as well as the two directions one to the other. 5.1.3.12 Detailing Requirements and Ductile Response There is a clear definition of the inter-relation between local detailing and local and global ductility of RC structures in EC8. For zones of low seismic exposure (say up to ground acceleration of 0.1g) ductility class L or M (low or medium) of EC8 may be used. Requirements for ductility class H (high) may be useful only in the case of structures where the designer requires a serious reduction in design forces, hence the use of an exceptionally high behaviour factor q. 5.1.3.13 Eurocode 8 Conceptual Design 544 Structural Engineering Analysis and Design Second Edition 545 Structural Engineering Analysis and Design Second Edition 546 Structural Engineering Analysis and Design Second Edition 5.1.4 Methods of Structural Analysis Earthquake excitations are random non-stationary functions starting from a low-level building up to a maximum then dying away. Exact solution methods are not established. Instead, we could either analyze a set of such events using either I. The Equivalent Lateral Force Response Spectrum method described in Section 5.1.5 (fundamental mode, linear, elastic analysis). This method automatically performs the seismic hazard assessment (of Section 5.1.1.18) and evaluates the effect of the soil layers (of Section 5.1.2.15.1) culminating in the response spectrum before the structural analysis is carried out. II. The Multi-Modal Response Spectrum method described in Section 5.1.5 (higher modes, linear, elastic analysis). This method automatically performs the seismic hazard assessment (of Section 5.1.1.18) and evaluates the effect of the soil layers (of Section 5.1.2.15.1) culminating in the response spectrum before the structural analysis is carried out. III. Performance Based Seismic Analysis and Design (a) Multi-Modal Response Spectrum (With No Behaviour Factor) methodology described in Section 5.1.5 and Section 5.1.10. (b) Random (Performance Based Seismic Engineering) solution method assuming a Gaussian and stationary (and ergodic) excitations as described in Section 4.6.4 and Section 5.1.10. This method requires the derivation of the input power spectrum (appropriately scaled to match the soil elastic response spectra) for the earthquake at soil level (from the seismic hazard assessment of Section 5.1.1.18 and effect of the soil layers of Section 5.1.2.15.1) to be applied onto the structure model or alternatively the input power spectrum (appropriately scaled to match the rock elastic response spectra) for the earthquake at rock level (from the seismic hazard assessment of Section 5.1.1.18) to be applied onto the soil and structure model. The latter soil and structure model clearly accounts for the soil-structure interaction (kinematic and inertial interaction) effect. (c) Deterministic Transient Solution (Performance Based Seismic Engineering) methods based on appropriately scaled (to match elastic response spectra) earthquake time histories and performing linear (as described in Section 4.8 and Section 5.1.10) or nonlinear (as described in Section 4.9 and Section 5.1.10) transient dynamic analyses and then enveloping the results (higher modes, nonlinear, inelastic analysis). This method requires the derivation of the input time histories (appropriately scaled to match the soil elastic response spectra) for the earthquake at soil level (from the seismic hazard assessment of Section 5.1.1.18 and effect of the soil layers of Section 5.1.2.15.1) to be applied onto the structure model or alternatively the input time histories (appropriately scaled to match the rock elastic response spectra) for the earthquake at rock level (from the seismic hazard assessment of Section 5.1.1.18) to be applied onto the soil and structure model. The latter soil and structure model clearly accounts for the soil-structure interaction (kinematic and inertial interaction) effect. 547 Structural Engineering Analysis and Design Second Edition 5.1.5 5.1.5.1 GL, ML Shock and Response Spectrum Analysis Nature of the Dynamic Loading Function The solution method can be used to solve dynamic systems subjected to: (a) Random non-stationary short duration impulse loading functions Deterministic loadings can be readily solved in the frequency or time domain using forced frequency and forced transient response analyses. Random loadings, which are stationary and ergodic, can be solved in the frequency domain using random vibration analysis. If the forcing function is a random non-stationary forcing function such that the random forces start from a low-level building up to a maximum then dying away, such as in a seismic event, then exact solution methods are not established. Instead, we could either analyze a set of such events using deterministic transient solution methods and then average or envelope the results or alternatively use the response or shock spectrum method which envelopes the response spectra of a series of time histories. The latter method, although computationally cheaper, ignores phase information of the signals. Response spectrum computes the relative response with respect to the base whilst shock spectrum computes the absolute response. In this LINEAR TIME DOMAIN solution, the static response must be added to the dynamic response if the dynamic analysis is performed about the initial undeflected (by the static loads) state with only the dynamic loads applied, hence causing the dynamic response to be measured relative to the static equilibrium position. Hence, the total response = the dynamic response + the static response to static loads. 5.1.5.2 The Response Spectra Response spectrum analysis is an approximate method of computing the peak response of a transient excitation applied to as simple structure or component. If is often used for earthquake excitations and also to predict peak response of equipment in spacecraft that is subjected to impulsive load due to stage separation. A response spectrum is a curve of the maximum response (displacement, velocity, acceleration etc.) of a series of single DOF systems of different natural frequencies and damping to a given acceleration time history. It 548 Structural Engineering Analysis and Design Second Edition characterizes the acceleration time history and has nothing to do with the properties of the structure. Any acceleration time series can be converted into a response spectrum. The response spectrum at rock level is obviously different from that on the soil surface because the acceleration time series would have been modified by the flexibility of the soil. Hence, the response spectrum is generated at the level where the structure stands. However, in doing so it becomes apparent that the characteristics of the soil no longer play any part in the dynamic response of the structure, i.e. there is no soil-structure interaction. The response spectrum gives the maximum response for a series of SDOF systems characterized by their natural frequencies and damping. To establish a response spectrum, the dynamic equations of motion are solved for each and every SDOF system using Duhamel’s integral for linear systems. Step-by-step linear acceleration method (explicit scheme since there is only one DOF) for nonlinear systems cannot really be employed, as superposition of nonlinear modal responses is not strictly valid for nonlinear systems where the physical coordinates (which includes all modes together) responds nonlinearly. One equation is solved for each SDOF system and the maximum value plots one point on the response spectra. When analyzing the dynamic response of a structure founded on rock, the input motion due to an earthquake is the same with or without the structure. Calculations assuming a fixed base structure should therefore give realistic results. However, when analyzing a structure founded on a soil site due to the same earthquake there are changes in motion at foundation level leading to changes in dynamic response of the structure. These changes are all effects of dynamic soil structure interaction. The structure will interact with the soil in two ways. Firstly, structural inertial loads are transferred back into the soil and secondly, the stiffer structural foundations are not able to conform to the generally non-uniform motion of the free-field surface. These effects are known respectively as inertial and kinematic interaction. To account for soil-structure interaction, other methods such as random solutions or deterministic transient solutions with both the soil and structure explicitly modeled must be employed. Once the response spectrum has been established, the response of a structure can be established depending on whether the idealization is SDOF (equivalent lateral force method) or MDOF (multi-modal spectrum analysis). 5.1.5.2.1 Ball Park Figures Wind loading base shear, Vwind = 0.01 – 0.03 WTOTAL Earthquake elastic base shear, Velastic = Se(g)(T1) WTOTAL = 0.25 – 0.30 WTOTAL in high seismicity areas Earthquake inelastic base shear, Vinelastic = Sd(g)(T1) WTOTAL = 0.15 – 0.20 WTOTAL in high seismicity areas = 0.05 – 0.07 WTOTAL in low seismicity areas Peak ground acceleration, PGA = 0.40g in high seismicity areas = 0.07g in low seismicity areas Spectrum amplification, M = 2.5 Se M T Behaviour factor, q = 2 for very non-ductile structures = 8.5 for very ductile structures 5.1.5.2.2 Low Period Structures T Spectral Acceleration Spectral Acceleration As RC structures crack with earthquake impact, T increases. Hence the spectrum is modified as follows. T 549 Structural Engineering Analysis and Design Second Edition 5.1.5.2.3 Behaviour Factors (Force Reduction Factors) for Inelastic Design It is not feasible, practical or economical to design elastically. The accelerations obtained from elastic loading Pe = Se(g)(T)W could cause great nonstructural damage and endanger lives as Se(T) >> Sd(T). The concept is to use the ductility of the structure to absorb energy by designing for Pd < Pe. Concepts of energy absorption in the inelastic range are used to reduce the elastic forces by as much as 80 – 85%. Hence the force reduction factor (aka response modification factor or behaviour factor) is Behaviour factor, q = Se Sd The relationships between elastic and inelastic forces for different periods are P P Pe=Pd Pe P Pe µ=δu/δy>δe/δy Pd δe=δu δ µ=δu/δy=δe/δy Pd δ Equal Acceleration δy δe Equal Energy Very Short Period Short Period Long Period T < 0.2s Pd = Pe 0.2s < T < 0.5s Pe Pd = 2µ − 1 T > 0.5s q = 2µ − 1 q=µ q = 1.0 δu δy δe=δu Equal Displacement Pd = δ Pe µ Hence, the behaviour factor depends on the period of the structure and to a lesser extent the period of maximum amplification in the earthquake spectrum. The force reduction factor q increases as T increases. The aspects that contribute to the value of q are I. Ductility i.e. inelastic energy absorption through damage, which is equivalent to having higher damping (accounted for) II. The ability of the structure to redistribute the action effects upon softening of a particular zone (accounted for) III. Loss of energy through radiation damping in the soil semi infinite half space (not accounted for) IV. Effect of uplift on cutting off the input of earthquake energy (not accounted for) The response modification (reduction) behaviour factor q is generally on the conservative side for the force calculations, but may be on the unconservative side for displacements. Hence, for the assessment of displacement, the linear elastic displacements under the design forces are multiplied (increased) by q to arrive to an approximate inelastic displacement. 550 Structural Engineering Analysis and Design Second Edition 5.1.5.2.4 UBC 1997 Elastic and Inelastic Response Spectrum The UBC elastic spectrum is defined by three lines governing low period response, mid period response and high period response. Depending on where the mode period T lands the base spectral acceleration Sa(g)(T) is defined by where T0 and T1 depend on the soil. The seismic coefficients Ca and Cv are dependent upon seismicity level and soil conditions at the site as follows. Na and Nu are near-source factors for Seismic Zone 4. Their values are in the range of 1.0 to 2.0 as follows. 551 Structural Engineering Analysis and Design Second Edition The zone factor Z represents the effective peak ground acceleration expected in the region and is in units of g. These values are obtained from seismic hazard analysis (as according to Section 5.1.1.18) culminating in the seismic zone map. The values reflect a 90% probability of not being exceeded in 50 years, which corresponds to a return period of 475 years. In the UBC, the US is divided into 5 seismic zones, namely, zones 1, 2A, 2B, 3, and 4. To account for the amplification effects introduced by different local soil conditions, the UBC distinguishes six different soil profile types as summarized as follows. In the absence of detailed information, one may assume type SD. Type SE or SF need not be considered unless it is substantiated by geotechnical investigations. The elastic spectrum can be converted into the inelastic spectrum by dividing by the ductility response modification factor, R. The structural factor R reflects the global ductility of the lateral load resistance system of the structure. The more ductile the structural system is, the lower can be the resistance of the structure and therefore, the larger can be the value of R. 552 Structural Engineering Analysis and Design Second Edition Criteria for Design The 1.4 x inelastic response spectrum is used for ultimate state plastic capacity design. To account for accidental torsional loads, where floor diagrams are not flexible, the UBC requires that the force Fi at each level be applied at a point that is away from the calculated center of mass by a distance that is 5% of the building dimension at that level perpendicular to the direction of Fi. where k = 5%. The UBC limits the story drift in a structure. The story drift, ∆ is the relative displacement between two adjacent levels of a structure. The drift ∆S is determined with the inelastic response spectrum. The maximum inelastic drift ∆M is then computed For structures with T < 0.7 seconds, For structures with T > 0.7 seconds, where H is the storey height. 553 Structural Engineering Analysis and Design Second Edition 5.1.5.2.5 EC8 Elastic and Inelastic Response Spectrum The elastic Se(g)(T) and inelastic spectrum Sd(g)(T) are defined in four parts as follows. The response spectrum is defined for 10% probability of occurrence in 50 years, or a return period of 475 years. The following depicts the horizontal response spectrum. Note that these response spectra are normalized by g. αSηβ0 SA (T) 1.0 αSηβ0/q αS 2/3 2.0 5/3 TB TC T (s) TD where the damping correction factor η with reference value η = 1 for 5% viscous damping is Note that α (or ag) is the peak ground acceleration in g, S is the soil response parameter, β0 is the spectral amplification factor for 5% damping, TB and TC are the limits of the constant acceleration region, TD is the limit of the constant displacement region and k1 and k2 are the spectrum shape exponents. The vertical response spectrum is obtained by scaling the horizontal response spectrum as follows. Note that the peak ground acceleration α (or ag) is the acceleration at bedrock level. This will be modified by the soil as depicted by the fact that at T = 0, the soil ground acceleration is αS. The soil would also affect the response spectrum for other values of T. The codified response spectra then represent the excitation signal at the soil level, and not at the bedrock level. A public domain database of the peak ground acceleration worldwide is maintained at GSHAP (http://www.seismo.ethz.ch/GSHAP/global/). The soil class determined parameters are as follows. 554 Structural Engineering Analysis and Design Second Edition Corresponding values of k1 and k2 for the elastic spectra are 1.0 and 2.0 for all subsoil classes. The subsoil classes are defined as follows. When the subsoil profile includes an alluvial surface layer with thickness varying between 5 and 20 m, underlain by much stiffer materials of class A, the spectrum shape for subsoil class B can be used together with an increased soil parameter S equal to 1.4, unless a special study is performed. Special attention should be paid in the case of a deposit of subsoil class C which consists — or contains a layer at least 10 m thick — of soft clays/silts with high plasticity index (PI > 40) and high water content. Such soils typically have very low values of vs, low internal damping and an abnormally extended range of linear behaviour and can therefore produce anomalous seismic site amplification and soil-structure interaction effects; In this case, a special study for the definition of the seismic action should be carried out, in order to establish the dependence of the response spectrum on the thickness and vs-value of the soft clay/silt layer and on the stiffness contrast between this layer and the underlying materials. Typically, the behaviour factor q is unity for elastic response and may be up to 5 for RC structures and 6 for steel structures. This may be contrasted with values of Rw but after dividing by 1.4 (i.e. Rw maximum is 12/1.4 = 8.5 and minimum 4/1.4 = 2.8) in recognition of the different philosophies consistent with the behaviour factor used. Note that when q is greater than about 2.5, the inelastic spectrum dips below the zero period value (ground acceleration). Of course, the greater the value of q, the lower the base shear. For concrete structures, q = q0kDkRkW. 555 Structural Engineering Analysis and Design Second Edition For steel structures q is given by the follows. 556 Structural Engineering Analysis and Design Second Edition For timber structures, the behaviour factor is listed 557 Structural Engineering Analysis and Design Second Edition 558 Structural Engineering Analysis and Design Second Edition For masonry structures, the behaviour factor is listed. For irregular buildings (in whatever material) q is further reduced by 20% from that listed above. The only difference between the elastic and the inelastic spectrum is the behaviour factor q and the values of k1 and k2. To be more precise, the spectral amplification β0 is divided by q in the inelastic spectrum. 559 Structural Engineering Analysis and Design Second Edition EC8 requires the dynamic mass calculated (i.e. divide the gravitational force by g to get mass) for the determination of the periods of the structure and the mass being acceleration by the ground motion (the greater the mass, the greater the base shear) from 100% DL + ϕψ2i LL where ϕ is obtained from The peak ground displacement may be estimated from The structural displacements can be determined from where q is the behaviour factor, de the displacement response and γ the importance factor. The importance factors are presented. 560 Structural Engineering Analysis and Design Second Edition Criteria for Design Seismic zones with a design ground acceleration α (i.e. peak ground acceleration in g) not greater than 0.10g are low seismicity zones, for which reduced or simplified seismic design procedures for certain types or categories of structures may be used. In seismic zones with a design ground acceleration α not greater than 0.04g the provisions of Eurocode 8 need not be observed. EC8 seismic load combinations cases are 1.0 DL + ψ2i LL ± γ 1.0 EQX 1.0 DL + ψ2i LL ± γ 1.0 EQY 1.0 DL + ψ2i LL ± γ 1.0 (EQX2 + EQY2)½ 1.0 DL + ψ2i LL ± γ 1.0 EQX ± γ 0.3 EQY ± γ 0.3 EQZ 1.0 DL + ψ2i LL ± γ 0.3 EQX ± γ 1.0 EQY ± γ 0.3 EQZ 1.0 DL + ψ2i LL ± γ 0.3 EQX ± γ 0.3 EQY ± γ 1.0 EQZ where ψ2i is obtained from the following table. EQ refers to the inelastic response spectrum. The enveloped results are employed to design the elements to its ultimate state plastic capacity. The EC8 limits the story drift in a structure. The inelastic displacement drift is obtained by multiplying the drift obtained from using the inelastic response spectrum by the behaviour factor. This value should not exceed 0.4% of the height of the story, H. ∆ d = q.∆ e < 0.004H ν 561 Structural Engineering Analysis and Design Second Edition where the reduction factor ν (accounting for the lower return period of the seismic event associated with the serviceability limit state) is Second order effects (P-∆ effects) need not be considered if the following condition is met for all storeys. If 0.1 < θ < 0.2, then P-∆ effects can be accounted for approximately by increasing seismic actions by 1/(1-θ). The value of θ shall not exceed 0.3. 562 Structural Engineering Analysis and Design Second Edition 5.1.5.2.6 IBC 2000 Elastic and Inelastic Response Spectrum The IBC spectrum is defined by three lines governing low period response, mid period response and high period response. The response spectrum Sa(g)(T) is defined where where the design spectral response acceleration parameters and where the maximum elastic spectra are where SS and S1 are the short period acceleration response parameter and the 1s period acceleration response parameter and the coefficients Fa and Fv which are dependent upon the site class and SS/S1 are defined The short period force reduction should normally be ignored in response spectrum calculations. 563 Structural Engineering Analysis and Design Second Edition 5.1.5.2.7 FEMA 356 Elastic and Inelastic Response Spectrum The FEMA 356 spectrum is defined by three lines governing low period response, mid period response and high period response. The response spectrum Sa(g)(T) is defined where where where SS and S1 are the short period acceleration response parameter and the 1s period acceleration response parameter and the coefficients Fa and Fv which are dependent upon the site class and SS/S1 are defined Site class D is default. The values for BS and B1 are a function of the effective viscous damping (β). Default value for β is 5%. The vertical response is 2/3 of the above response spectrum. 564 Structural Engineering Analysis and Design Second Edition 5.1.5.3 GL, ML SDOF Response Spectrum Analysis – Equivalent Lateral Static Force Method The equivalent lateral force method is a special case of the multi-modal approach, i.e. by only including the fundamental mode. A SDOF system subject to base excitations, in relative terms has the following ODE. m& u&r ( t ) + cu&r ( t ) + ku r ( t ) = − m& u&s ( t ) The response will be obtained in relative terms as follows from Duhamel’s (Convolution) Integral. u r (τ = t ) u r max (τ = t ) τ= t = 1 mω d ∫ = 1 mω d ∫ = 1 ωd = 1 MAX  ωd  = 1 Sv ωd ∫ τ= 0 τ= t τ= 0 τ= t τ =0 p(τ)e − ξωn ( t − τ) sin ω d ( t − τ)dτ − m& u&s (τ)e −ξωn ( t − τ) sin ω d ( t − τ)dτ −& u&s (τ)e −ξωn ( t − τ ) sin ω d ( t − τ)dτ ∫ τ= t τ=0 & u&s (τ)e −ξωn ( t − τ) sin ω d ( t − τ)dτ  where S v = pseudo spectral velocity Because of the irregularity of the excitation function, the Duhamel’s Integral will have to be solved numerically. The plot of the maximum dynamic displacement response urmax for various natural periods Ti is known as the spectral displacement (or the displacement response spectrum), SD. The spectral velocity (or the velocity response spectrum) is SV and the spectral acceleration is SA. These are related approximately as follows. S S V = ω n ,d S D = A ω n ,d It is a mere coincidence that these relationships are same as that between acceleration, velocity and displacement in simple harmonic motion. The derivation of the response spectrum enables the response prediction of SDOF systems. For a SDOF system, the maximum dynamic force (i.e. the base shear) on the SDOF mass is then Max dynamicforce = ku rmax = k SV S = mω 2n V ωd ωd ≈ mω n S V W SA g ≈ WSA (g) ≈ If the structure is idealized as a SDOF system characterized by its first fundamental frequency or period T1, the response is computed as follows (i) (ii) (iii) (iv) The fundamental period T1 of the structure corresponding to the horizontal first mode is established The response is computed in g ms-2 from the response spectrum SA(g)(T1) The base shear is computed as Fbase shear = SA(g)(T1)W The base shear is distributed linearly along the height of the structure and a static analysis performed; this effectively determines the equivalent dynamic response Note that in the equation for base shear V = SA(g)W, the acceleration spectrum SA(g) is in terms of g. Also, W is the modal weight, i.e. the modal mass times g. Here in the equivalent static force method, we only consider the fundamental period. Noting for most structures, the fundamental modal weight W1 is some 80-90% of the total 565 Structural Engineering Analysis and Design Second Edition weight, if the spectral ordinates SA1 is larger or equal to SA2, SA3 etc …, then replacing W1 by WT will always yield an upper bound on V. SA(g) SA(g) S1A(g) S2B(g) S2A(g) S2A(g) T2A T1A T T2B T T1B Since S1A is multiplied by W1, which is normally much larger than W2, W3 etc …, then multiplying S1A by WT will yield an upper bound on the total force. This is clearly not the case for system B. The equivalent lateral static force method is very crude since it does not consider higher (than the fundamental) modes of vibration, and hence is not really a dynamic analysis. Higher modes may be significant especially at the local level even if they do not contribute much to the base shear. This is simply because higher modes have shapes which are fundamentally different from that of the fundamental mode cause localized higher forces. Higher modes can be addressed by performing the multi-modal method. We have said that the base shear is V = WTSA(g). Codes of practice generally provide methods of calculating this expression. This expression then of course account for the fundamental mode only, but the response spectra derived from codes of practice can be used for the multi-modal spectrum analysis. Now, for this fundamental mode approach (equivalent lateral load), codes of practice state V = SA(g)WT. Typically SA(g) depends on I. II. III. IV. V. Period dependent coefficient representing the shape of the spectrum Importance factor representing the probability of the design load being exceeded Zone factor representing the seismic hazard at the site Site response parameter representing the amplification characteristic of the soil Response modification factor representing the ability of the structure to dissipate energy 566 Structural Engineering Analysis and Design Second Edition 5.1.5.3.1 UBC 1997 For Seismic Zones 3 and 4, the static load procedure is only applicable to regular structures under 240 ft. in height or irregular structures not more than five stories or 65 ft. in height. The equivalent lateral force < < W is the total weight of the structure. The UBC further requires that for Seismic Zone 4, I is the structural importance factor. The base shear is distributed based on which is based on the assumption that the fundamental mode of the structure has a linear shape. Ft is the top storey force to account for higher mode effects. The force at each level is proportional to the height and story weight. Clearly, the total base shear is In general, higher-mode effects are only important for structures that have relatively long fundamental periods. Hence, in the UBC, Ft is zero when T < 0.7 seconds and it increases in proportion to T up to 0.25V, i.e. 567 Structural Engineering Analysis and Design Second Edition The fundamental period T can be obtained using the empirical formula where hN is the height of the building in feet as follows Alternatively, it can be obtained using modal analysis or Rayleigh’s formula 1 T1 = 2π g ∑W δ ∑W δ i 2 i i i Although the latter method is more rational, the UBC requires that the value of T obtained with the modal analysis or Rayleigh’s method be no greater than that obtained with the empirical by more than 30% for Seismic Zone 4 and 40% for Seismic Zones 1, 2, and 3. 5.1.5.3.2 EC8 Base shear, Fb = Sd(T1).W Fundamental period of vibration, T1 = CtH0.75. Alternatively, it can be obtained using modal analysis or Rayleigh’s formula 1 T1 = 2π g ∑W δ ∑W δ i 2 i i i The base shear is assumed linearly distributed along the height of the building, hence the seismic forces at level i are given by Fi where zi is the height of the storey from the ground. z .W Fi = Fb . i i z j .W j ∑ 5.1.5.3.3 IBC 2000 The base shear is where 568 Structural Engineering Analysis and Design Second Edition < < For buildings in Seismic Design Category E or F where S1 > 0.6g, Cs must be greater than The fundamental period of the structure is calculated as where the factor CT depends on the type of building frame and hN is the height of the building in feet. Alternatively the fundamental period of the building can be calculated from a modal analysis, but cannot exceed where Cu is a function of SD1 (the design response acceleration at 1 second period). The vertical force is distributed as follows. where where the exponent k depends on the building period from 1 for buildings with a short period to 2 for buildings with a long period. Fx is the force applied at each storey, this is then distributed across the nodes on the storey in proportion to the nodal masses. 5.1.5.3.4 FEMA 356 The base shear is given by The fundamental period is calculated from The factors CT and β depend on the type of building frame and h is the height of the building in feet. Alternatively, the fundamental period can be calculated from modal analysis. The vertical distribution of forces is given by where where the exponent k depends on the building period from 1 for buildings with a short period to 2 for buildings with a long period. Fx is the force applied at each storey, this is then distributed across the nodes on the storey in proportion to the nodal masses. 569 Structural Engineering Analysis and Design Second Edition 5.1.5.4 GL, ML MDOF Response Spectrum Analysis – Multi-Modal Seismic Analysis For a MDOF system, the equation of motion for support excitation in relative terms is [M ]{& u&( t )} + [C]{u&( t )} + [K ]{u ( t )} = −[M ]{1}& u&s ( t ) Note that {D} = {1} is a unity vector corresponding to the rigid body motion. The support excitation causes all the masses to produce an inertial force opposing its motion (D’Alembert’s Principle). Let {u ( t )} = [Φ ]{ξ( t )} [M ][Φ ] & ξ&( t ) + [C][Φ ] ξ&( t ) + [K ][Φ ]{ξ( t )} = −[M ]{1}& u&s ( t ) { } { } Premultiplying by [Φ ] reduces the coupled system of ODEs to a system of uncoupled ODEs T T T [Φ ]T [M ][Φ] & ξ&( t ) + [Φ ] [C][Φ ] ξ&( t ) + [Φ ] [K ][Φ ]{ξ( t )} = −[Φ ] [M ]{1}& u& ( t ) T { } { } [M]{& ξ&( t )}+ [C]{ξ&( t )}+ [K ]{ξ( t )} = −[Φ ] [M ]{1}& u& ( t ) s T s Each uncoupled equation being T M i& ξ&i ( t ) + C i ξ&i ( t ) + K i ξ i ( t ) = −{φ i } [M ]{1}& u&s ( t ) Dividing the equation of motion for the ith natural mode from above by its modal mass gives T Mi & ξ&i ( t ) + C i ξ&i ( t ) + K i ξ i ( t ) = −{φ i } [M ]{1}& u&s ( t ) − {φ i } [M ]{1}& u&s ( t ) 2ξ M ω K & ξ&i ( t ) + i i ni ξ&i ( t ) + i ξ i ( t ) = Mi Mi Mi 2 & & & ξ ( t ) + 2ξ ω ξ ( t ) + ω ξ ( t ) = Γ & u& ( t ) T i i ni i ni i i s where the ith mode participation factor is defined as Γi = − {φ i }T [M ]{1} =− Mi {φ i }T [M ]{1} {φ i }T [M ]{φ i } Bereft of the modal participation factor, the equations of motion reduce to simple SDOF systems characterized by only the natural frequency and damping and subject to the excitation & u&s ( t ) . Duhamel’s Integral is used to evaluate numerically to derive the response spectra to & u&s ( t ) . That is to say, for & q&i ( t ) + 2ξ i ω ni q&i ( t ) + ω 2ni q i ( t ) = & u&s ( t ) the response is q r (τ = t ) = 1 mω d = 1 mω d = 1 ωd ∫ ∫ τ= t τ =0 ∫ τ= t τ =0 τ= t τ= 0 p(τ)e −ξωn ( t − τ) sin ω d ( t − τ)dτ − m& u&s (τ)e −ξωn ( t − τ) sin ω d ( t − τ)dτ −& u&s (τ)e − ξωn ( t − τ) sin ω d ( t − τ)dτ τ= t 1 & MAX  u&s (τ)e − ξωn ( t − τ ) sin ω d ( t − τ)dτ ωd  τ =0  1 Sv where S v = pseudo spectral velocity = ωd q r max (τ = t ) = ∫ 570 Structural Engineering Analysis and Design Second Edition The plot of the maximum dynamic displacement response for various natural periods Ti is known as the spectral displacement (or the displacement response spectrum), SD i.e. qrmax. The spectral velocity (or the velocity response spectrum) is SV and the spectral acceleration is SA. These are related approximately as follows. S S V = ω n ,d S D = A ω n ,d It is a mere coincidence that these relationships are same as that between acceleration, velocity and displacement in simple harmonic motion. The maximum modal responses are then ξ i max ( t ) = Γi S D ξ& ( t ) = Γ S i max i V & ξ&i max ( t ) = Γi S A Once the individual maximum modal responses are computed, the maximum physical responses is calculated from the following based on some method of superposition. {u rmax (t)} = [Φ ]{ξ max ( t )} {u& (t)} = [Φ ]{ξ& ( t )} rmax max {& u&rmax (t)} = [Φ ]{& ξ&max ( t )} Thus, if the structure is idealized as a MDOF system characterized by its first few frequencies or period T1, the response spectrum analysis method is performed as follows. (i) The response spectrum is first established from the forcing acceleration time history. The acceleration response of a notional mode (of a particular natural frequency) is established separately from solving the equation of motion bereft of the modal participation factor & q&i ( t ) + 2ξ i ω ni q&i ( t ) + ω 2ni q i ( t ) = & u&s ( t ) resulting in the solution for each notional mode (each natural frequency) in the time domain by Duhamel’s Integral 1 τ= t q r (τ = t ) = −& u&s ( τ)e − ξωn ( t − τ ) sin ω d ( t − τ)dτ ω d τ=0 ∫ the maximum of which is found for each notional mode (each natural frequency) to define the (maximum) response spectra τ= t 1 & S D = q r max ( τ = t ) = MAX  u&s ( τ)e −ξωn ( t − τ ) sin ω d ( t − τ)dτ ωd  τ=0  ∫ S V = ω n ,d S D = (ii) SA ω n ,d The modal (or generalized) mass Mi is computed for each mode i as follows Mi = {φi}T[M]{φi} The actual magnitudes of the modal masses in itself are incomplete to describe the importance of the mode (as the amplitude of the modal force must also be considered) as they depend on the method of eigenvector normalization 571 Structural Engineering Analysis and Design Second Edition (iii) The amplitude of the modal force is for each mode i Li = {φi}T[M]{1} where the vector {D} = {1} simply represents the vector of rigid body motion. (iv) And the modal participation factor and effective mass for each mode i is defined as Modal participation factor, Γi = Li / Mi Modal effective mass, EffectiveMassi = Li2 / Mi both representing the relative contribution of each mode (excluding the frequency content of the excitation function which is encapsulated in the response spectrum) to the response prior to multiplication by the input function. The fundamental mode shape will usually have a dominant participation factor and effective mass associated with it. Higher modes will have a lower participation because the positive and negative components of the mode shape in the participation expression cancels out. This generally does not occur in load excitations unless the loading is uniformly distributed, such as is the case in enforced motion. Sufficient modes must be included such that ∑Li2/Mi is at least 90% of the total mass. Participation factor and modal effective mass is calculated in NASTRAN using the Case Control Command MEFFMASS. (v) The maximum modal response in modal space for mode i is computed as follows ξ i max ( t ) = Γi S D ξ& ( t ) = Γ S i max i V & ξ&i max ( t ) = Γi S A (vi) The maximum modal responses in physical space for mode i is then computed as follows {u imax (t)} = {φ i }ξ i max ( t ) = {φ i }Γi S D {u& (t)} = {φ }ξ& ( t ) = {φ }Γ S imax i i max i i V {& u&imax (t)} = {φ i }& ξ&i max ( t ) = {φ i }Γi S A (vii) The (dynamic) base shear for a particular mode i is Vi = EffectiveMass i SA = [{φ } [M]{1}] S T 2 i {φi }T [M]{φi } A If SA is expressed as a fraction of g, then the modal base shear is Vi = EffectiveWeight i S A (g ) [{φ } [W]{1}] S = T 2 i {φi }T [W ]{φi } A (g ) Hence, for a simple building of floors denoted by m, the modal base shear for mode i is 2  m=all   w m φ mi    S (g ) Wi =  mm==1all A w m φ 2mi ∑ ∑ m =1 572 Structural Engineering Analysis and Design Second Edition (viii) Finally the modal force response (i.e. force at every DOF) for mode i is computed as follows {Fi } = [M]{& u&i (t)} = [M ]{φ i }Γi S A {φ }T [M ]{1} S = [M ]{φ i } i T {φi } [M]{φi } A 2 T [ M ]{φ i } [{φ i } [M ]{1}] = S {φi }T [M]{1} {φi }T [M]{φi } A [M]{φi } V = {φi }T [M]{1} i The above can also be expressed in weight ratios as {Fi } = [WT ]{φi } Vi {φ i } [W ]{1} Hence, for a simple building of floors denoted by m, the force at floor m due to mode i is f mi = Vi M m φ mi m =all ∑M = Vi m φ mi w m φ mi m = all ∑w m =1 (ix) m φ mi m =1 The modal responses are then combined using the SRSS or the CQC combinations. The upper bound responses of the different modes can be established using the SRSS method if the modal frequencies are well separated. Alternatively, the complete quadratic combination (CQC) method should be used if some modal frequencies are closely spaced, in which case the absolute sum of the response of these closely spaced modes is taken on the assumption that they can peak in phase with each other. These combinations can be used for any modal response, be it the displacement, velocity, acceleration, modal force responses or modal base shears. SRSS : V = n ∑V 2 i i =1 CQC : V = n n ∑∑ Vi β ij Vj βij = i =1 j=1 (1 − r ) 2 2 ( ) (ζ 8 ζiζ j 1/ 2 ( i ) + rζ j r1.5 ) ( ) + 4ζ i ζ j r 1 + r 2 + 4 ζ i2 + ζ 2j r 2 The cross-modal parameters βij are a function of the duration and frequency content of the earthquake record, and frequencies and damping characteristics of the structure. For an earthquake duration much longer than the periods of the structure and a response spectrum which is not exceptionally spiky and constant modal damping, the cross-modal parameters are given by βij = 8ζ 2 (1 + r )r1.5 (1 − r ) 2 2 + 4ζ 2 r(1 + r ) 2 where ζ is the damping ratio and r is the period ratio (Ti/Tj). Indeed, the use of CQC is recommended in general, but the difference between the two methods diminishes rapidly as the mode spacing increases. 573 Structural Engineering Analysis and Design Second Edition The assumptions and limitations of a multi-modal response spectrum analysis are as follows: (i) (ii) (iii) (iv) (v) (vi) The response spectrum method only provides the maximum values of response. The analysis is geometrically and materially linear and the nonlinearity is very crudely incorporated into the analysis using the q-factor (Europe) to reduce the amplitudes of the elastic response spectra to an inelastic response spectra. Higher modes are accounted for, i.e. the interstorey forces generated due to higher modes are taken into account by computing the modal displacement responses and converting that to the modal force responses. These are then applied as static forces in a linear static analysis. We can say that the dynamic effects of higher modes are effectively taken into account, however only if the response is linear and elastic. An alternative would be to perform nonlinear time domain analyses of appropriately scaled (to match response spectra) seismic time histories and envelope the results. Since the response spectrum is the maximum response of a series of SDOF systems, it must be remembered that the peak response for one SDOF system does not occur at the same time as the peak response for another. In other words there is no phase information between the responses of the individual modes or SDOF systems. Hence, various methods to combine these peak responses are employed such as the SRSS (Square Root of the Sum of the Squares), the ABS (absolute values) the NRL (U.S. Navy Shock Design Modal Summation) or the CQC (complete quadratic combination). Thus, the results of a response spectrum analysis are not a set of results in equilibrium but the maximum values that can be expected. There is also no consideration of phase of the response with respect to the loading as only the magnitude is computed. Another restriction of the response spectrum method is that it is only valid if all support motion in a given direction is identical. This is usually valid for ground movements applied to buildings or local floor movements applied to equipment but it is not applicable to piping systems where the anchor points of the pipe are connected to different structures or even different parts of the same structure 9. Another case would be a long span suspension bridge where the earthquake excitations may differ on either side of the abutment. It is assumed that each oscillator mass is very small relative to the base structural mass so that the oscillator does not influence the dynamic behavior of the base structure, i.e. no soil-structure interaction accounted for in the earthquake vibration analysis. If base isolation is employed, the stiffness of the base isolator can be incorporated into the finite element model, hence elongating the periods. Base isolation in effect simply introduces a low frequency component into the system. The periods will be elongated and the corresponding response spectra value will be lower. Base isolation is thus used for stiff structures in order to elongate the effective period of the system. 9 NAFEMS. A Finite Element Primer. NAFEMS Ltd., Great Britain, 1992. 574 Structural Engineering Analysis and Design Second Edition 5.1.5.4.1 UBC 1997 The design base shear determined from the multi modal response shall not be less than 90% of that determined by the equivalent static load procedure for regular structures and 100% for irregular structures. Hence there is a requirement for a scale factor for the force as follows Vequivalent static 1 but Force scale factor = α T Force scale factor > R Vmulti − mod al where αT is 0.9 for regular structures or 1.0 for irregular structures. Likewise the scale factor for displacements Vequivalent static Displacement scale factor = α T Vmulti − mod al 5.1.5.4.2 EC8 No additional specific requirements. 5.1.5.4.3 IBC 2000 No additional specific requirements. 5.1.5.4.4 FEMA 356 No additional specific requirements. 575 Structural Engineering Analysis and Design Second Edition 5.1.5.5 Example Application EC8 Following a seismic hazard of Section 5.1.1.18 and the soil response analyses of Section 5.1.2.15.1, a peak ground acceleration at the bedrock level of 0.6g and at the soil level of 0.15g has been obtained. The results of these two initial steps culminate in the response spectra. The 0.15g acceleration corresponds to the value of the response spectrum at period, T = 0.0s. The soil analysis will also produce ordinates of the response spectrum for other values of the period, T. With this, the seismic action effects on the structure are determined based on the simplified equivalent lateral force analysis and the multi-modal response spectrum analyses. The level of member detailing corresponds to ductility class “M” and the site soil conditions are such that soil class “B” is appropriate. The regularity of the structure in plan enables the analysis to be based on a typical frame as shown below. The floor slabs are assumed to be infinitely rigid (i.e. no large openings etc.) in order to distribute the floor shear forces amongst the columns in diaphragm action. 3m 3m 3m 6m 5.1.5.5.1 6m 6m 6m Structural Loading Assume a concrete volumetric weight of 25 kN/m3. Loads on Slabs Self-weight of slab + partitions, G = 6 kN/m2 Live load, Q = 3 kN/m2 Loads on Beams Dead load on beam, Gk = self-weight + slab dead load x width = 0.3 x 0.5 x 25 + 6 x 5 = 33.75 kN/m Live load on beam, Qk = slab live load x width = 3 x 5 = 15 kN/m 5.1.5.5.2 Seismic Forces Using the Simplified Equivalent Lateral Force Analysis of EC8 Fundamental Period of Vibration Using Simplified Method Fundamental period of vibration, T1 = CtH0.75 = 0.075 x H0.75 = 0.075 x 90.75 = 0.39s Fundamental Period of Vibration Using Rayleigh’s Method Seismic self weight on storey 3: Gk + ΨE Qk = 33.75 x 24 + 0.3 x (15 x 24) = 918 kN (no column) Seismic self weight on storey 2: Gk + ΨE Qk = 918 + 5 x 0.4 x 0.5 x 3 x 25 = 993 kN Seismic self weight on storey 1: Gk + ΨE Qk = 993 kN A structural static analysis programme was used to give the displacement of the structure under the seismic weight as shown in below. 576 Structural Engineering Analysis and Design Second Edition Cross-sectional Properties Beam Column Area bd = 30 x 50 = 1500 cm2 bd = 50 x 40 = 2000 cm2 Second moment of area about major axis 1/12bd3 = 1/12 x 30 x 503 = 312500 cm4 1/12bd3 = 1/12 x 40 x 503 = 416667 cm4 Second moment of area about minor axis 1/12db3 = 1/12 x 50 x 303 = 112500 cm4 1/12db3 = 1/12 x 50 x 403 = 266667 cm4 0.070m 918 kN 0.053m 993 kN 0.024m 993 kN 6m T1 = 2π 1 g ∑W δ ∑W δ 2 i i i i 6m = 2π 6m 1  918x 0.070 2 + 993x 0.053 2 + 993x 0.024 2  9.81  918x 0.070 + 993x 0.053 + 993x 0.024 6m   = 0.47s   The fundamental period of the structure calculated from both the simplified method and Rayleigh’s method are very similar. This is because the structure is uniform and regular. The low period also signifies a relatively stiff structure, which is why the simplified method provided an accurate estimate. Behaviour Factor The behaviour factor represents the ability of the structure to respond in a ductile manner. Higher values of q require greater level of detailing for ductility. However, the greater energy absorbing capacity provided by the greater ductility enables the structure to be designed for lower seismic action forces. The behaviour factor q reduces as T increases, but dependence on the period is not explicitly considered. Also, over-strength and redundancy parameters are not taken into account either. Behaviour factor, q = q0 kD kR kW where basic behaviour factor, q0 = 5.0 as this is a RC frame system kD = 0.75 as this is a ductility class “M” structure kR = 1.0 as this is a regular structure kW = 1.0 as this is a frame system Hence, q = 5 x 0.75 x 1 x 1 = 3.75 577 Structural Engineering Analysis and Design Second Edition Inelastic Spectral Acceleration of EC8 From previous soil response analysis of Section 5.1.2.15.1, (i) (ii) the soil at the site is characterized by shear wave velocities of 200 to 250 m/s at depths of 10m and 450 to 500 at depths of 50m. This signifies Soil Class “B”. Hence, S = 1.0, β0 = 2.5, TB = 0.15 and TC = 0.6. design ground acceleration in terms of g, α = 0.15 Also, because the structure is of reinforced concrete, the critical viscous damping ζ is 5%. Hence, η = (7/(2+ζ))0.5 = 1. The linear elastic response spectrum is reduced by the behaviour factor q in order to force the structure to resist the seismic actions in the inelastic range. This allows for the design based on lower seismic design forces.. Elastic and Design Spectra of EC8 TB TD TC 0.4 0.35 0.3 0.25 0.2 0.15 0.1 0.05 0 Se Sd 0 0.5 1 1.5 2 2.5 3 3.5 4 4.5 Period T (s) Spectral acceleration, Sd (T1 ) = α.S.η. β0 , q = 0.15 x 1.0 x 1.0 x TB ≤ T1 ≤ TC 2.5 3.75 = 0.1g Base Shear Base shear, Fb = Sd(T1).W = 0.1 x (918 + 993 + 993) = 290.4 kN Seismic Forces Per Storey Assuming that the base shear is linearly distributed along the height of the building, the seismic forces at level i are given by Fi where zi is the height of the storey from the ground. Fi = Fb . z i .Wi z j .W j ∑ z3 = 3m, z2 = 6m, z1 = 9m ΣzjWj = 3 x 993 + 6 x 993 + 9 x 918 = 17199 kNm Seismic force at Level 3, F1 = 290.4 x (9 x 918) / 17199 = 139.5 kN Seismic force at Level 2, F2 = 290.4 x (6 x 993) / 17199 = 100.6 kN Seismic force at Level 1, F3 = 290.4 x (3 x 993) / 17199 = 50.3 kN 578 Structural Engineering Analysis and Design Second Edition Level 3 F1 = 139.5 kN Level 2 F2 = 100.6 kN z1 Level 1 F3 = 50.3 kN z2 z3 5.1.5.5.3 Seismic Loads using Multi-Modal Analysis The flexibility matrix of the 3 storey shear frame model is obtained from the structural static analysis program by successively applying 1kN unit loads at each storey and each time measuring the total displacement at all the storey levels. Flexibility Matrix  f1,1  F =  f 2,1 f  3,1 f1, 2 f 2,2 f 3, 2 f1,3   0.040 0.024 0.009     f 2,3  =  0.024 0.022 0.009  mm/kN f 3,3   0.009 0.009 0.007  The slab contribution to the flexural capacity of the frame has been neglected in that the effective width of the top flange of the beams is taken as the width of the web of the beam. Hence in reality, the slab would actually provide a slightly stiffer response to that predicted. Stiffness Matrix 18.109   73.441 − 87.525   K = F −1 =  − 87.525 200.201 − 144.869   18.109 − 144.869 305.835    18109   73441 − 87525   =  − 87525 200201 − 144869   18109 − 144869 305835    Mass Matrix 0 0   93.578   M= 0 101.223 0   0 0 101.223   kN / mm kN / m tonnes The mass matrix is the seismic weight at each level as calculated includes the full dead load and 30% of the live load. Eigenvalues ω2 To find ω2, we solve the eigenvalue equation  K - ω2 M  = 0  73441 − 93.578ω 2  K − ω2 M =  − 87525  18109  − 87525 200201 − 101.223ω 2 − 144869  18109   − 144869 2 305835 − 101.223ω  579 Structural Engineering Analysis and Design Second Edition Hence the eigenvalue equation is given by:  K - ω2 M  = 0.1006036 x 1016 − 0.6718900 x 1013 ω2 + 0.5545779 x 1010 ω4 − 958809.146 ω6 = 0  ω12   173.959      ω 2 =  ω 22  =  1449.824   2     ω3   4160.245  ωI represents the fundamental natural circular frequency of this structure as it is the smallest. This gives the fundamental mode shape and the fundamental period. Mode Shapes φ The equation [ K - ω i2 M ][φ i] = 0 is solved for i = 1 to 3 to give the three different mode shapes. [K − ω M ][φ ] = [0] 2 i i for i = 1, 2, 3 Normalising the first row to unity, [ φ = φ1 φ2 1 1   1  φ 3 = 0.715 − 0.906 − 2.840 0.297 − 0.939 3.726  ] φ1 is the fundamental mode shape, i.e. the shape that requires the least amount of energy to vibrate. Modal Mass (Generalized Mass), Participation Factor and Effective Mass It is necessary to compute the contribution of each mode of vibration to the response of the structure. To this end the effective mass, which represents the structure as a single-degree-of-freedom system, is computed. Modal mass (generalized mass) GMi = φiT M φi, modal force amplitude Li = φiT M{1}, effective mass mi = Li 2 / GMi for i = 1 to 3 0 0  1   93.578    GM = φ Mφ = (1 0.715 0.297 ) 0 101.223 0  0.715  = 154.215  0 0 101.223  0.297   1T 1 1 0 0 1  93.578    L = φ M{1} = (1 0.715 0.297 ) 0 101.223 0 1 = 195.959  0 0 101.223 1  1T 1 2 L1 195.959 2 m = = = 249.0 154.215 GM1 1 2T GM = φ Mφ 2 2 = (1 − 0.906 0 0  1   93.578    0 101.223 0  − 0.906  = 265.846  0 0 101.223  − 0.939   − 0.939 ) 0 0 1  93.578    L = φ M{1} = (1 − 0.906 − 0.939 ) 0 101.223 0 1 = -93.141  0 0 101.223 1  2 2T 2 m2 = L2 - 93.1412 = = 32.6 2 265.846 GM 580 Structural Engineering Analysis and Design Second Edition 0 0  1   93.578    GM = φ Mφ = (1 − 2.840 3.726 ) 0 101.223 0  − 2.840  = 2315.248  0 0 101.223  3.726   3T 3 3 0 0 1  93.578    L = φ M{1} = (1 − 2.840 3.726 ) 0 101.223 0 1 = 183.271  0 0 101.223 1  3T 3 2 L3 183.2712 m = = = 14.5 GM 3 2315.248 3 Hence, GM = [154.215 265.846 2315.248] L = [195.959 − 93.141 183.271] m = [249 32.6 14.5] = [84% 11% 5%] The effective mass associated with the fundamental mode of vibration, m1 is clearly the largest at 84% of the total mass, and hence the forces imparted upon the structure vibrating in this fundamental mode are the most damaging (i.e. the critical case). Natural Periods of Vibration  T1   0.48   2π    T= =  T2  =  0.17  seconds ω      T3   0.10  The fundamental period is 0.48 seconds. Inelastic Response Spectrum of EC8 From previous soil response analysis of Section 5.1.2.15.1, (i) Subsoil class “B”. Hence, S = 1.0, β0 = 2.5, TB = 0.15 and TC = 0.6. (ii) Design ground acceleration in terms of g, α = 0.15 Also, because the structure is of reinforced concrete, the critical viscous damping ζ is 5%. Hence, η = (7/(2+ζ))0.5 = 1. The behaviour factor q = 3.75, as before. Spectral acceleration, S d (T1 = 0.48) = α.S.η. β0 q TB ≤ T1 ≤ TC = 0.15 x 1.0 x 1.0 x 2.5 3.75 = 0.100g Spectral acceleration, S d (T2 = 0.17) = α.S.η. β0 q TB ≤ T2 ≤ TC = 0.15 x 1.0 x 1.0 x 2.5 3.75 = 0.100g 581 Structural Engineering Analysis and Design Second Edition  T  β Spectral acceleration, S d (T3 = 0.10) = α.S.1 + 3 .(η. 0 − 1) , 0 ≤ T3 ≤ TB q  TB  2.5  0.10  = 0.15 x 1.0 x 1 + .(1 x − 1) 0 . 15 3 . 75   = 0.117g Modal Force Response The modal force responses are the horizontal loads at each level for the different mode shapes. Li S e ,i GM i f i = Mφ i for i = 1 ,2, 3 0 0  1   93.578 116.6     195.959   L1 f1 = M φ Sd ,1 =  0 101.223 0  0.715  0.100 x 9.81 =  90.2  kN GM1 154.215  0  37.4  0 101.223  0.297     0 0  1   93.578  − 32.2     - 93.141   2 L2 f 2 = Mφ Sd , 2 =  0 101.223 0  − 0.906  0.100 x 9.81 =  31.5  kN GM 2 265.846  0  32.7  0 101.223  − 0.939     0 0  1   93.578  8.5     183.271   3 L3 f 3 = Mφ Sd,3 =  0 101.223 0  − 2.840  0.117 x 9.81 =  − 26.1 kN GM 3 2315.248  0  34.3  0 101.223  3.726     1 8.5  116.6 − 32.2   f =  90.2 31.5 − 26.1 kN  37.4 32.7 34.3   Modal Combination using SRSS As the natural periods of vibration are not too closely spaced between the different modes, the Square Root of the Sum of Squares, SRSS, is used to combine the modal responses providing a reasonable estimate of the total maximum response. ff j = ∑ i ∆= F − ff F f j2,i 121.3    =  99.0  kN  60.4    13.0    x100% =  1.6  %  20.1   Since this structure is regular, higher modes of vibrations are rather insignificant. The fundamental period is also less than 2, hence the simplified equivalent lateral force analysis method is sufficient. 582 Structural Engineering Analysis and Design Second Edition 5.1.5.5.4 Structural Static Analysis A structural static analysis is now carried out using the forces computed with the simplified equivalent lateral force and the vertical loads, given by 1.0 Gk + 0.3 Qk, shown in below. The next two figures show the bending moment and the shear force diagrams. -38.3 kN/m -38.3 kN/m -38.3 kN/m -38.3 kN/m -38.3 kN/m -41.4 kN/m -41.4 kN/m -41.4 kN/m -41.4 kN/m -41.4 kN/m -41.4 kN/m -41.4 kN/m -41.4 kN/m -41.4 kN/m -41.4 kN/m 140 kN 101 kN 50.3 kN Loading 49.4 kNm 159 kNm 83.3 kNm 147 kNm 81.9 kNm 148 89.3kNm kNm 127 kNm 193 kNm 59.2 kNm 188 kNm 62 kNm 186 kNm 61.4 kNm 185 kNm 45.6 kNm 12 kNm 90.9 kNm -67 kNm 129 kNm -62.5 kNm 126 kNm -61.9 kNm 126 kNm -83.5 kNm 136 kNm Bending Moment Diagram 133 kN 125 kN 126 kN 33.1 kN -96.5 kN -104 kN -104 kN -108 kN 149 kN -58.3 kN -103 kN 146 kN 145 kN 33.1 3.6 kN kN -99.6 kN -104 kN -104 kN 154 kN -58.3 kN -101 kN 148 kN -62.9 kN -100 kN 148 kN 3.6 -26.3 kNkN -94.4 kN -26.3 kN -62.9 kN Shear Force Diagram 583 -102 kN 121 kN -66.9 kN 145 kN -66.9 -72.6 kN 147 kN -72.6 -73.3 kN -73.3 kN Structural Engineering Analysis and Design Second Edition 5.1.5.5.5 Serviceability Limit Verification The displacements computed in the analysis, shown below, are used to verify that the serviceability limit has not been exceeded. 8.6 mm 6.0 mm 2.5 mm Horizontal Displacements EC8 sets limits on the deformation that is allowed at each level under seismic action. This relative displacement (drift) should not exceed 0.4% of the height of the story, thus for each storey of the structure this drift should not exceed 12mm. The figure shows the displacements at each level: Storey 3: ∆r = 0.0086-0.0060 = 0.0026m (< 0.012m) Storey 2: ∆r = 0.0060-0.0025 = 0.0035m (< 0.012m) Storey 1: ∆r = 0.0025-0.0000 = 0.0025m (< 0.012m) What we have here is the elastic displacement due to the inelastic forces, however this is unacceptable for design purposes. To obtain the inelastic displacements these elastic displacements are multiplied by the behaviour factor, q. This gives: Storey 3: ∆r = 0.0026 x 3.75 = 0.00975m (< 0.012m) Storey 2: ∆r = 0.0035 x 3.75 = 0.01313m (> 0.012m) Storey 1: ∆r = 0.0025 x 3.75 = 0.00938m (< 0.012m) Hence on the second storey the drift fractionally exceeds the limit, however the analysis does not take into account the stiffness of the slab. Therefore this design is probably satisfactory but may entail slight adjustments to the section in question. 584 Structural Engineering Analysis and Design Second Edition 5.1.5.6 MSC.NASTRAN Decks There are two parts to a response spectrum analysis, namely the generation of the spectrum and the use of the spectrum to compute the dynamic response. The response spectrum analysis is the only dynamic analysis method that requires a SUPORT entry to define the input DOFs for the spectra. The procedure involves two stages. First the applied loads or base excitations are converted in a direct transient solution (SOL 109) into a spectrum table consisting of peak response magnitudes for a set of single degree-offreedom oscillators. Each oscillator is a scalar spring/mass/damper having a different natural frequency and damping ratio. This stage is optional since the shock spectrum data is frequently given in the contractual design specifications or, in the case of earthquakes, is available through governmental agencies. The second stage of the analysis consists of a modal analysis of the structure, data recovery, and the response calculation that combines the modal properties of the analysis model with the spectrum data of the applied loads. This stage is performed in a modal analysis solution sequence (SOL 103). If a database was saved from the first stage, a restart will provide the spectrum data automatically. Otherwise, the spectrum data must be supplied in a direct tabular input (response versus natural frequency for several damping ratios). 5.1.5.6.1 Theoretical Background 585 Structural Engineering Analysis and Design Second Edition 586 Structural Engineering Analysis and Design Second Edition 5.1.5.6.2 Response Spectra Generation Response spectra are generated in the transient response solution sequences (SOL 109 for direct and SOL 112 for modal). Transient response input is required to apply the transient excitation to the base structure. Additional input is described. Relative and absolute spectra are denoted by IP and RM, respectively, in the parentheses of the curve request. There are two FREQi entries: one to specify oscillator frequencies (i.e., frequencies for which spectra will be computed) and the other to specify oscillator damping. (Note that damping for the base structure is specified in another manner, such as with the TABDMP1 entry used for modal transient response analysis.) 5.1.5.6.3 Peak Response Calculation Response spectrum application is a postprocessing function of normal modes analysis (SOL 103). It is run in the normal modes solution sequences, so the modelling and analysis considerations that apply for normal modes analysis also apply for response spectrum application. The additional considerations also need to be followed: 1. The structure is run as an unrestrained model in the direction(s) of the load spectrum application. 2. A large mass, on the order of 103 to 106 times the mass of the structure, must be used at the structure’s base grid points where the input occurs. One way to do this is to use RBEs or MPCs to connect the base points to a separate grid point, and apply the large mass to that separate grid point. This separate grid point is where the spectrum is applied. 3. A SUPORT Bulk Data entry is required at the spectrum input location. 4. The modes must be mass normalized (which is the default). The spectra that MSC.Nastran can apply are absolute acceleration, relative displacement, and relative velocity spectra. You specify A, D, or V for acceleration displacement or velocity, respectively, to specify the spectrum type. Use all modes within the frequency range specified by the spectrum, but do not use modes outside of the 587 Structural Engineering Analysis and Design Second Edition spectrum range. Usually, spectra to apply are considered to have zero values outside of their range of definition; for example, an absolute acceleration spectrum defined from 0 to 30 Hz is assumed to be zero beyond 30Hz. However, MSC.Nastran extrapolates spectral values for modes beyond the spectral range, which may lead to unexpected answers. You can limit the number of modes used in the spectrum application by limiting the number of computed modes (via the EIGRL or EIGR entry) or by using PARAM,HFREQ,r (where r is the highest frequency mode to use) or PARAM,LMODES,n (where n is the number of lowest modes to use). Consider the entire response spectrum process—generation and application—as a two-step process. Step 1 is generation of the response spectra and Step 2 is the application of the response spectra. For a given input, transient applied to the base structure (Step 1), the same stresses occur (Step 2) regardless of whether acceleration or displacement spectra were computed in Step 1. However, displacements and accelerations are different, because answers computed by using the absolute acceleration spectrum contain the rigid body contribution, whereas answers computed by using the relative displacement spectrum do not contain the rigid body contribution. Displacement and acceleration responses can be made equal regardless of which spectra was used by using PARAM,LFREQ,0.01 (or some other small number) to remove the rigid body mode contribution from the answers. Stresses and other element quantities are unaffected by the contribution of any rigid body modes. The same situation applies to relative velocity spectra as to relative displacement spectra. All input listed in the table is required with the exception of PARAM,OPTION and PARAM,CLOSE. The time step (field 4 on the TSTEP Bulk Data entry, DT) should not be changed during the run, because MSC.Nastran uses only the initial DT specification for the entire response spectrum generation run and therefore wrong answers could occur. The time step, DT, and time duration, (where is the number of time increments), must take into account the loading, the base structure, and the frequency range of the spectra generation. The time step must take into account the frequency content of the applied excitation, the frequencies of the base structure, and the highest frequency for which spectra are to be generated. There must be enough time steps per cycle of response for both the base structure and the highest frequency oscillator in order to accurately predict the peak response; 5 to 10 steps per cycle represent a typical value. In addition, the time duration of the loading, the frequencies of the base 588 Structural Engineering Analysis and Design Second Edition structure, and the lowest oscillator frequency must be considered when defining the time duration. There must be a long enough time duration of response both for the base structure and the lowest frequency oscillator in order to accurately predict the peak response. For short duration loadings, the peak response often occurs well after the load has peaked. Initial conditions (specified via the TIC Bulk Data entry) are not used in response spectrum generation. Initial conditions are used in the calculation of the transient response of the base structure, but the calculation of the peak oscillator responses (i.e., the response spectrum calculation) ignores any initial conditions. 589 Structural Engineering Analysis and Design Second Edition 5.1.6 Reinforced Concrete Design to EC8 for Earthquake Effects Based on Response Spectrum Analysis 5.1.6.1 Concepts of Ductility The definition of ductility is µ= Deformation Quantity at Ultimate Deformation Quantity at Yield The deformation considered may be curvature µφ, rotation µθ, or displacement µδ, commonly the latter. 5.1.6.1.1 Section Ductility Curvature ductility, µ φ = φ u / φ y where φy = yield of reinforcement - higher As, Asv, and fy would increase ductility as φy decreases - Asv increases confinement hence increasing ductility where φu = ultimate compressive strain of concrete, i.e. concrete crushing - higher axial load increases compressive strain, hence decreasing ductility as φu decreases 5.1.6.1.2 Member Ductility Displacement ductility, µ ∆ = ∆u θ and Rotation ductility, µ θ = u ∆y θy where ∆y = yield of reinforcement - higher As, Asv, and fy would increase ductility as ∆y decreases where ∆u = ultimate compressive strain of concrete, i.e. concrete crushing or buckling or fracture of rebars - higher axial load increases P-∆ effects, hence decreasing ductility as ∆u decreases - higher levels of Asv will decrease risk of buckling of rebars, hence increasing ductility by increasing ∆u - strain hardening rebars will promote spread of inelasticity, hence lengthening the plastic hinge length, increasing ductility as ∆u increases 5.1.6.1.3 Structural Ductility Structural ductility = Total drift at top of structure / Total base shear or Structural ductility = behaviour factor q = ability to achieve inelastic deformations I. Capacity design concepts should be employed. The structure is viewed comprising of dissipative and nondissipative parts. The dissipative zone mobilizes desired failure mode and avoids collapse and maximizes the energy dissipation. (a) The dissipative zones are dimensioned first and carefully detailed to posses maximum ductility (b) Their likely sources of over-strength is estimated:- higher concrete compressive strength, fcu - higher yield strength of steel, fy - larger area of steel rebars, As - slab contribution to effective flange compressive area in the case of beams - confinement - strain-hardening characteristics of steel (c) The non-dissipative parts are then designed to withstand forces consistent with the strength of dissipative parts, including over-strength. Hence the non-dissipative parts do not reach MP i.e. its plastic capacity until the dissipative parts have reached MP and absorbed considerable energy through ductility. II. Continuity and redundancy between members to ensure clear load path III. Regularity of mass, stiffness and strength distribution to avoid torsional effects and soft-storeys IV. Reduced mass V. Sufficient stiffness to avoid highly flexible structures with significant P-∆ effects and non-structural damage. 590 Structural Engineering Analysis and Design Second Edition 5.1.6.2 Capacity Design for Optimum Location and Sequence of Attainment of Member Capacity Whereas in static design, under-estimating the member strength is an added safety procedure, this is not the case in seismic design. This is because the location and sequence of attainment of member capacity are very important for the collapse prevention and optimum response, respectively. Location of attainment of MP Hinges should form in beams and not columns in order to avoid an unstable mechanism that will lead to collapse. Sequence of attainment of MP Using the ductility of elements to absorb energy instead of the yield strength is a more optimum method. MC1 We thus require beam hinges and not column hinges. Except at the base of the column, hinges are not accepted anywhere else on the column. The method of utilizing capacity design is as follows MC2 MB Obtain the structural member forces from structural analysis of the earthquake excitation I. Design beam to resist MB II. Estimate the over-strength of the beam, the sources of which are fc, fy, As, slab contribution; Say MBactual = 1.25MB III. Scale up MC1 and MC2 to satisfy equilibrium with 1.25MB. If the column stiffness were equal, then MC1=MC2=0.625MB instead of 0.5MB. IV. Hence, the beam plastic hinge will definitely occur first, and the energy will then be absorbed by the ductility of the member. The plastic capacity of the columns won’t be reached; instead the mechanism collapses when the ductility limit of the beam has been attained. 5.1.6.3 Capacity Design for Favourable Mechanism of Deformation Flexural deformation is the more favourable mechanism of dissipation of energy than shear deformation because it is more ductile. To ensure flexural deformation precedes shear deformation, consider the design for a cantilever. P M Shear cracking Flexural cracking 1. Design M=PL, hence design beam for bending capacity M=PL. 2. Estimate over-strength of Mactualcapacity = 1.25M = 1.25PL. 3. Design beam for shear force in equilibrium with 1.25PL, i.e. Vdesign = 1.25PL. A point to note is that having strain hardening steel rebars is favourable for an efficient bending deformation energy dissipating mechanism. Perfectly plastic rebars will cause the formation of only one flexural crack. Hence the plastic hinge length will be short and hence the ductility requirement at that section is considerable. Strain hardening rebars will cause the formation of many flexural cracks. Hence the plastic hinge length will be long and hence the ductility requirement per section along the hinge length is reduced. The latter represents a far more efficient energy dissipating mechanism. In the case of RC walls, the shear force consistent with the flexural strength, increased by a factor of about 20% in recognition of i) unintentional increase in steel yield fy, ii) round up of As, iii) strain hardening of flexural reinforcement and iv) additional fcu, is used to determine the shear capacity needed. Hence, flexural failure precedes shear failure. 591 Structural Engineering Analysis and Design Second Edition 5.1.6.4 Introduction of Example Problem Following the determination of the seismic action, the reinforced concrete beams and columns are now designed. The design of the beams is based on EC2, which governs the design of concrete structures, and that of the columns is based on EC8, which makes provisions for the earthquake resistance of structures. The regularity of the structure in plan enables the analysis to be based on a typical frame as shown below. The floor slabs are assumed to be infinitely rigid (i.e. no large openings etc.) in order to distribute the floor shear forces amongst the columns in diaphragm action. 3m 3m 3m 6m 5.1.6.5 6m 6m 6m Design Data Material used for design: Concrete class C25/30, longitudinal steel S400, transverse steel S220 Concrete cover to reinforcement is 30mm. ⇒ Concrete design strength, fcd = 25/1.5 = 16.7MPa ⇒ Longitudinal steel strength, fyd = 400/1.15 = 347.8MPa ⇒ Transverse steel strength, fyd = 220/1.15 = 191.3MPa 5.1.6.6 5.1.6.6.1 Beam Design for Vertical Loading According to EC2 Structural Loading Assume a concrete volumetric weight of 25 kN/m3. Initial sizing of beam, web = 0.3m, depth = 0.5m from previous project. Loads on Slabs Self-weight of slab + partitions, G = 6 kN/m2 Live load, Q = 3 kN/m2 Loads on Beams Dead load on beam, Gk = self-weight + slab dead load x width = 0.3 x 0.5 x 25 + 6 x 5 = 33.75 kN/m Live load on beam, Qk = slab live load x width = 3 x 5 = 15 kN/m 592 Structural Engineering Analysis and Design Second Edition 5.1.6.6.2 Determination of Maximum Action Effects The maximum bending moment is calculated for the different combinations of 1.35G + 1.5Q. The following gives the maximum elastic bending moment in the spans and the maximum elastic bending moment in the supports. The range of values for both the moments in the spans and the supports is not very large so only one beam needs to be designed for the entire structure. MAXIMUM BENDING MOMENT IN SPANS WITH 1.35G+1.5Q 1.35G + 1.5Q 1.35G + 1.5Q 1.0G 1.0G 1.0G 1.35G + 1.5Q 1.35G + 1.5Q 1.0G 1.35G + 1.5Q 1.35G + 1.5Q 1.0G 1.0G LOADING DIAGRAM Max: 194 kNm Max: 189 kNm Max: -121 kNm Max: -130 kNm Max: 191 kNm Max: 192 kNm Max: -117 kNm Max: -117 kNm Max: 196 kNm Max: 195 kNm Max: -113 kNm Max: -117 kNm BENDING MOMENT DIAGRAM 593 Structural Engineering Analysis and Design Second Edition MAXIMUM BENDING MOMENT IN SUPPORT 1.35G 1.35G 1.35G 1.35G 1.35G 1.35G 1.35G 1.35G 1.35G 1.35G 1.35G 1.35G LOADING DIAGRAM 221 kNm 203 kNm 206 kNm 193 kNm 207 kNm 206 kNm 202 kNm 182 kNm 211 kNm 203 kNm 206 kNm 157 kNm BENDING MOMENT DIAGRAM 594 Structural Engineering Analysis and Design Second Edition SEISMIC LOADCASE G+0.3Q+E 1.0G + 0.3Q 140 kN -33.8 kN/m -4.5 kN/m 1.0G + 0.3Q -33.8 kN/m 101 kN -4.5 kN/m 1.0G + 0.3Q -33.8 kN/m 50.3-4.5 kN kN/m 1.0G + 0.3Q -33.8 kN/m -4.5 kN/m -33.8 kN/m -4.5 kN/m 1.0G + 0.3Q -33.8 kN/m -4.5 kN/m 1.0G + 0.3Q -33.8 kN/m -4.5 kN/m 1.0G + 0.3Q -33.8 kN/m -4.5 kN/m 1.0G + 0.3Q -33.8 kN/m -4.5 kN/m 1.0G + 0.3Q 1.0G + 0.3Q -33.8 kN/m -4.5 kN/m 1.0G + 0.3Q -33.8 kN/m -4.5 kN/m -33.8 kN/m -4.5 kN/m -33.8 kN/m -4.5 kN/m 1.0G + 0.3Q -33.8 kN/m -4.5 kN/m -33.8 kN/m -4.5 kN/m 89.6 kNm 126 kNm Max: 126 kNm LOADING DIAGRAM 160 kNm Max: 160 kNm 147 kNm Max: 147 kNm 83.4 kNm 48.7 kNm Max: -58.4 kNm Max: -72.4 kNm Max: -64.6 kNm 183 kNm Max: 183 kNm 179 kNm Max: 179 kNm 176 kNm Max: 176 kNm 177 kNm Max: 177 kNm 52.6 kNm 49.7 kNm 51.5 kNm 37.4 kNm Max: -63.9 kNm Max: -63.3 kNm Max: -63.7 kNm Max: -69.5 kNm 196 kNm Max: 196 kNm 186 kNm Max: 186 kNm 186 kNm Max: 186 kNm 182 kNm Max: 182 kNm 44 kNm 44.2 kNm 43.1 kNm 18.8 kNm Max: -64.4 kNm Max: -64.8 kNm Max: -66 kNm Max: -76.1 kNm BENDING MOMENT DIAGRAM FOR BEAMS 595 Structural Engineering Analysis and Design Second Edition 48.7 kNm 31.8 kN -40.3 kN -34.5 kN -30.9 kN -65.6 kN 70.4-106 kNm kNm 31.8 0.387kNkN -40.3 -58.1 kN kN -34.5 -56.2 kN kN -30.9 -56.8 kN kN -65.6 -69.4 kN 102-79.9 kNmkNm 0.387 -28.2 kN -58.1 -65.4 kN -56.2 -62.9 kN -56.8 -62.4 kN -69.4 -71.4 kN -28.2 kN -65.4 kN -62.9 kN -62.4 kN -71.4 kN -76.2 kNm -65.2 kNm -58.4 kNm -126 kNm -9.31 -46.7kNm kNm 44.7 -89.1 kNm kNm 38.2 -88.1 kNm kNm 34.4 -90.2 kNm kNm 8.38 -10.5kNm kNm 85.1 -67kNm kNm 80.4 -62.5 kNm kNm 80.3 -61.8 kNm kNm 92.8 kNm 129 kNm 126 kNm 126 kNm 134 kNm BENDING MOMENT DIAGRAM FOR COLUMNS -96.3 kN -90.4 kN -85.2 kN 133 kN 125 kN 126 kN -104 kN -104 kN -109 kN 139 kN 136 kN 135 kN -93.2 kN -94.2 kN -93.9 kN 144 kN 138 kN 139 kN -91.1 kN -90.9 kN -91.8 kN SHEAR FORCE DIAGRAM FOR COLUMNS 121 kN 96.3 kN 237 kN 229 kN 234 kN 121 kN 136 kN 96.3 187 kN kN 237 470 kN 229 460 kN 234 464 kN 121 256 kN 138 kN 187 272 kN 470 705 kN 460 689 kN 464 694 kN 256 394 kN 272 kN 705 kN 689 kN 694 kN 394 kN AXIAL FORCE DIAGRAM FOR COLUMNS 596 Structural Engineering Analysis and Design Second Edition 5.1.6.6.3 Design for Bending Redistribution Redistribution is carried out in order to optimise the design by obtaining a more uniform distribution of the action effects. The maximum value of the bending moment is 221 kNm. The redistribution is to be carried out for each beam. First a 15% redistribution is applied, i.e. δ = 0.85: MSd = 0.85 x 221 = 187.85 kNm First the normalised moment, µ, is calculated: µ= M Sd bd 2 f cd x 187.85 = 0.17 ⇒ Table 1 ⇒ = 0.28 2 3 d 0.3 × 0.47 × 16.7 × 10 x The condition stipulated in EC2 is that δ ≥ 0.44 + 1.25 . This is to ensure that the beam is adequately ductile. d Since 0.44+1.25x0.28 = 0.79, is less than 0.85, so the design can proceed, taking maximum support moments of 187.85 kNm. ⇒ µ= To find the maximum moments in the midspan after redistribution: 2 2  M R − M L pλ   − 187.85 + 160 68.1 × 6  +  +    λ 2 6 2     + M max = M L + = −160 + = 132.7 kNm 2p 2 × 68.1 New values of the maximum shear force can be checked by taking moments about the support. In general this does not make a difference, e.g. the maximum value of 215kN was reduced to 210kN. These changes are negligible. Design of Longitudinal Positive Reinforcement (i) Effective width, bef = 0.3 + 0.2 x (0.85 x 6) = 1.32 m M 132.7 (ii) Normalised moment, µ, is calculated: µ = 2Sd = = 0.027 bd f cd 1.32 × 0.47 2 × 16.7 × 103 From Table 110 ⇒ ω = 0.028; ξ = 0.084 (iii) Check if the neutral axis depth is within the section’s flange: x = 0.084 x 0.47 = 0.039 m (< 0.12m) bdf cd 1.32 × 0.47 × 16.7 (iv) The area of steel is calculated: A s = ω = 0.028 × ≅ 8.34 cm 2 f yd 347.8 From Table 2 ⇒ 6φ14 (9.24cm2) (v) Detailing checks: The minimum area of reinforcement is given as 0.0015bd = 2.25 cm2 ⇒ OK The maximum area of reinforcement is given as 0.04Ac = 60 cm2 ⇒ OK Design of Longitudinal Negative Reinforcement (i) Effective width, bef = bw = 0.3m (ii) Normalised moment, µ, is calculated: µ = 10 M Sd 187.85 = = 0.170 2 bd f cd 0.3 × 0.47 2 × 16.7 × 10 3 CEB 1992 597 Structural Engineering Analysis and Design Second Edition From Table 111 ⇒ ω = 0.192; ξ = 0.280 (iii) The area of steel is calculated: A s = ω bdf cd 0.3 × 0.47 × 16.7 = 0.192 × ≅ 13.00 cm 2 f yd 347.8 From Table 2 ⇒ 7φ16 (14.07cm2) (iv) Detailing checks: The minimum area of reinforcement is given as 0.0015bd = 2.25 cm2 ⇒ OK The maximum area of reinforcement is given as 0.04Ac = 60 cm2 ⇒ OK 5.1.6.7 Capacity Check for Seismic Loading of Beams Actual moment capacity of positive reinforcement = Asfyd(d-x/2) = 924 x 347.8 x (470-39/2) = 144.776 x 106 Nmm = 144.7 kNm Actual moment capacity of negative reinforcement = Asfyd(d-x/2) = 1407 x 347.8 x (470-131.6/2) = 197.8x106 Nmm = 197.8 kNm The required moments for the seismic action-effects are 196 kNm at the support and 72.4 kNm at the span, which are lower than the actual capacities as calculated above. 11 CEB 1992 598 Structural Engineering Analysis and Design Second Edition 5.1.6.8 Design of Transverse Reinforcement The maximum shear force, VSd = 215kN, at the internal support of the left beam on the top floor is due to the vertical load case. The seismic load combination is only 144kN, so we design for the vertical load case, hence we use EC2. The design value of 215kN can be reduced to 215 - ρd = 183kN which corresponds to the shear force at a distance d from the support. 5.1.6.8.1 Check Maximum Design Force That Can Be Carried Without Crushing of Concrete VSd = 183kN VRd2 = maximum design force that can be carried without crushing of concrete VRd2 = 0.5νfcdbw x 0.9d where ν = (0.7-fck/200) = 0.575 ≥ 0.5 VRd2 = 608.1 kN > 183kN ⇒ OK, there is no increase of dimensions required. 5.1.6.8.2 Check If Shear Reinforcement Is Required VRd1 = design shear of a member without shear reinforcement VRd1 = [τRdk(1.2+40ρ1)+0.15σcp]bwd τRd = 0.035fck2/3 = 300kPa k = 1.6-d = 1.13, however, much of the bottom reinforcement will be curtailed before the supports (only 30% extends into the support) and thus does not contribute to shear resistance, so k will be taken as unity. π × 16 2 π × 14 2 7× + 2× A 4 4 ρ= s = = 0.012 (≤ 0.02 ) bwd 300 × 470 σ cp ≈ 0 So, VRd1 = [300x1x(1.2+40x0.012)] x 0.3 x 0.47 =71 kN (<183kN) Since VRd1 < VSd the beam requires shear reinforcement. 5.1.6.8.3 Design Required Shear Reinforcement Vwd = VSd - VRd1 = 183 – 71 = 112kN The shear reinforcement is given by the following equation, where As and s are unknown: A sw Vwd 112 ≥ = = 1.38mm 2 / mm s 0.9df ywd 0.9 × 0.47 × 191.3 Assuming a diameter of 10 mm, remembering that there are two links across the section, the maximum spacing is 114 mm. So, choose shear links, φ10@110mm 5.1.6.8.4 ⇒ ⇒ Check Code Limits 1/5 x 608 = 121.6 kN; 2/3 x VRd2 = 405.3kN 1/5VRd2 < VSd < 2/3VRd1 The spacing of the transverse reinforcement should not exceed the lesser of the following three distances: a) 12 x the minimum diameter of the longitudinal bars = 12 x 14 = 168mm b) the least dimension of the column = 300mm c) 300mm ⇒ OK 599 Structural Engineering Analysis and Design Second Edition 5.1.6.9 Column Design The seismic load case is clearly the critical combination of actions for the columns. So this combination will be used for the design of the columns. Initial size of columns assumed from previous project as 500x400 mm. 5.1.6.9.1 M-N Pairs and Normalised Actions M N The normalised actions are given by: µ = 2Sd ; ν = Sd bhf cd bh f cd ωtot is obtained from the M-N interaction diagrams Internal Column Storey Seismic N (kN) 3 2 1 237 470 705 M (kNm) 76.2 89.1 129 µ ν ωtot Static N (kN) 0.0456 0.0534 0.0772 0.057 0.113 0.169 0.080 0.030 0.060 419 830 1243 µ ν ωtot Static N (kN) 0.0754 0.0635 0.0802 0.029 0.061 0.094 0.180 0.060 0.100 194 395 595 M (kNm) 74 47.7 60.5 µ ν ωtot 0.0443 0.0286 0.0362 0.100 0.199 0.298 0 0 0 µ ν ωtot 0.0940 0.0605 0.0484 0.046 0.095 0.143 0.16 0.02 0 External Column Storey Seismic N (kN) 3 2 1 121 256 394 M (kNm) 126 106 134 M (kNm) 157 101 80.9 The minimum total reinforcement ratio, ρtot, allowed by the code is 1%. This corresponds to a mechanical ratio, ωtot,min = ρtot (fyd/fcd) = 0.01(347.8/16.7) = 0.208, which is larger than all the values calculated. Therefore the minimum requirement is used to determine the reinforcement areas for both exterior and interior columns: 1 A S1 = A S 2 = ω tot bh f cd / f yd = 0.5 × 0.208 × 2000 × (16.7 / 347.8) = 10 cm 2 2 Two 22 mm bars, one at each corner, and one intermediate 20 mm bar provide adequate reinforcement for the columns on each side. The total area is 27.8 cm2 and the total reinforcement ratio is 1.4%. ( ) In theory, the columns should be redesigned to give a more economical solution since they are being controlled by the minimum reinforcement requirements. However, this would result in the breaking of code limits so minimum requirements dominate in both the exterior and the interior columns. Hence, one standard column design is used for both interior and exterior columns with minimum nominal steel reinforcement. 600 Structural Engineering Analysis and Design Second Edition 5.1.6.9.2 Capacity Design Considerations The following calculations are based on the seismic load case 1.0G + 0.3Q + 1.0E. Exterior Beam-Column Joints For ductility class ‘M’, γRd = 1.2 a) For direction '1' of seismic action, the top of the beam is in tension (i) actual beam moment capacity, M Rd = 182 x (14.07/13.00) = 197 kNm (ii) sum of moments ratio, α CD1 = γ Rd = 1.2 x (iii) the moment reversal factor, δ1 = M lR1 + M rR1 M So1 + M Su1 0 + 197 = 1.30 102 + 79.9 M Sr 1 − M Sl 1 + M rR1 M lR1 = 0 − 182 0 + 197 = 0.92 (iv) capacity design requirement, M Sd1,CD = 1 + (α CD,1 − 1)δ1 M Sd1 o column over joint, M Sd1, CD = 1 + (1.30 − 1)0.92 (102) = 130.2 axial load acting on column above joint, N o = −256kN, hence ν = −0.08 reinforcement ratio for one side of column, ρ1 = ( ) 2π22 2 / 4 + π20 2 / 4 = 0.0054 400 × 500 hence, ω tot = 2ρ1 f yd / f cd = 0.224 giving from interaction diagram design charts, µ = 0.12 thus, M oRd = µbh 2 f cd = 0.12 × 0.4 × 0.5 2 × 16.7 × 10 3 = 200.4 > M oCD = 130.2 thus there is no need to change the column reinforcement. u column under joint, M Sd1, CD = 1 + (1.30 − 1)0.92 (79.9) = 102.0 axial load acting on column under joint, N u = −394kN, hence ν = −0.12 reinforcement ratio for one side of column, ρ1 = ( ) 2π22 2 / 4 + π20 2 / 4 = 0.0054 400 × 500 hence, ω tot = 2ρ1 f yd / f cd = 0.224 giving from interaction diagram design charts, µ = 0.13 u thus, M uRd = µbh 2 f cd = 0.13 × 0.4 × 0.5 2 × 16.7 × 10 3 = 217.1 > M CD = 102.0 thus there is no need to change the column reinforcement. 601 Structural Engineering Analysis and Design Second Edition b) For direction '2' of seismic action, the top of the beam is still in tension (i) actual beam moment capacity, M Rd = 18.8 x (14.07/13.00) = 20.3 kNm M lR 2 + M rR 2 (ii) sum of moments ratio, α CD 2 = γ Rd M So 2 + M Su2 = 1.2 x (iii) the moment reversal factor, δ 2 = 0 + 20.3 = 1.29 10.5 + 8.38 M Sr 2 − M Sl 2 M rR 2 + M lR 2 = 0 + 18.8 0 + 20.3 = 0.93 (iv) capacity design requirement, M Sd2,CD = 1 + (α CD , 2 − 1)δ 2 M Sd 2 o column over joint, M Sd2, CD = 1 + (1.29 − 1)0.93 (10.5) = 13.3 axial load acting on column above joint, N o = −187kN, hence ν = −0.06 reinforcement ratio for one side of column, ρ1 = ( ) 2π22 2 / 4 + π20 2 / 4 = 0.0054 400 × 500 hence, ω tot = 2ρ1 f yd / f cd = 0.224 giving from interaction diagram design charts, µ = 0.115 thus, M oRd = µbh 2 f cd = 0.115 × 0.4 × 0.5 2 × 16.7 × 10 3 = 192.1 > M oCD = 13.3 thus there is no need to change the column reinforcement. u column under joint, M Sd2, CD = 1 + (1.29 − 1)0.93 (8.4) = 10.7 axial load acting on column under joint, N u = −272kN, hence ν = −0.08 reinforcement ratio for one side of column, ρ1 = ( ) 2π22 2 / 4 + π20 2 / 4 = 0.0054 400 × 500 hence, ω tot = 2ρ1 f yd / f cd = 0.224 giving from interaction diagram design charts, µ = 0.12 u thus, M uRd = µbh 2 f cd = 0.12 × 0.4 × 0.5 2 × 16.7 × 10 3 = 200.3 > M CD = 10.7 thus there is no need to change the column reinforcement. 602 Structural Engineering Analysis and Design Second Edition Interior Beam-Column Joints For ductility class ‘M’, γRd = 1.2 a) For direction '1' of seismic action, the top of the beam is in tension (i) actual beam moment capacity, M lRd = 1 96 x (14.07/13.00) = 212.1 kNm M rRd = 44 x (14.07/13.00) = 47.6 kNm (ii) sum of moments ratio, α CD1 = γ Rd = 1.2 x (iii) the moment reversal factor, δ1 = M lR1 + M rR1 M So1 + M Su1 212.1 + 47.6 = 2.05 67 + 85.1 M Sr 1 − M Sl 1 M rR1 + M lR1 = − 44 − 196 47.6 + 212.1 = 0.92 (iv) capacity design requirement, M Sd1,CD = 1 + (α CD,1 − 1)δ1 M Sd1 o column over joint, M Sd1, CD = 1 + (2.05 − 1)0.92 (85.1) = 167.3 axial load acting on column above joint, N o = −470kN, hence ν = −0.15 reinforcement ratio for one side of column, ρ1 = ( ) 2π22 2 / 4 + π20 2 / 4 = 0.0054 400 × 500 hence, ω tot = 2ρ1 f yd / f cd = 0.224 giving from interaction diagram design charts, µ = 0.15 thus, M oRd = µbh 2 f cd = 0.15 × 0.4 × 0.5 2 × 16.7 × 10 3 = 250.5 > M oCD = 167.3 thus there is no need to change the column reinforcement. u column under joint, M Sd1, CD = 1 + (2.05 − 1)0.92 (67 ) = 131.7 axial load acting on column under joint, N u = −705kN, hence ν = −0.21 reinforcement ratio for one side of column, ρ1 = ( ) 2π22 2 / 4 + π20 2 / 4 = 0.0054 400 × 500 hence, ω tot = 2ρ1 f yd / f cd = 0.224 giving from interaction diagram design charts, µ = 0.17 u thus, M uRd = µbh 2 f cd = 0.17 × 0.4 × 0.5 2 × 16.7 × 10 3 = 283.9 > M CD = 131.7 thus there is no need to change the column reinforcement. 603 Structural Engineering Analysis and Design Second Edition b) For direction '2' of seismic action, the top of the beam is still in tension (i) actual beam moment capacity, M lRd = 1 86 x (14.07/13.00) = 201.3 kNm M rRd = 44.2 x (14.07/13.00) = 47.8 kNm (ii) sum of moments ratio, α CD 2 = γ Rd M lR 2 + M rR 2 M So 2 + M Su2 = 1.2 x (iii) the moment reversal factor, δ 2 = 201.3 + 47.8 = 2.1 80.3 + 61.8 M Sr 2 − M Sl 2 M rR 2 + M lR 2 = 186 + 44.2 201.3 + 47.8 = 0.92 (iv) capacity design requirement, M Sd2,CD = 1 + (α CD , 2 − 1)δ 2 M Sd 2 o column over joint, M Sd2, CD = 1 + (2.1 − 1)0.92 (80.3) = 161.6 axial load acting on column above joint, N o = −464kN, hence ν = −0.14 reinforcement ratio for one side of column, ρ1 = ( ) 2π22 2 / 4 + π20 2 / 4 = 0.0054 400 × 500 hence, ω tot = 2ρ1 f yd / f cd = 0.224 giving from interaction diagram design charts, µ = 0.15 thus, M oRd = µbh 2 f cd = 0.15 × 0.4 × 0.5 2 × 16.7 × 10 3 = 250.5 > M oCD = 161.6 thus there is no need to change the column reinforcement. u column under joint, M Sd2, CD = 1 + (2.1 − 1)0.92 (61.8) = 124.3 axial load acting on column under joint, N u = −694kN, hence ν = −0.21 reinforcement ratio for one side of column, ρ1 = ( ) 2π22 2 / 4 + π20 2 / 4 = 0.0054 400 × 500 hence, ω tot = 2ρ1 f yd / f cd = 0.224 giving from interaction diagram design charts, µ = 0.17 u thus, M uRd = µbh 2 f cd = 0.17 × 0.4 × 0.5 2 × 16.7 × 10 3 = 283.8 > M CD = 124.3 thus there is no need to change the column reinforcement. This capacity check ensures that the plastic hinge will occur in the beams before it occurs in the columns. Hence, the formation of the plastic hinge in the beam will lead to a stable mechanism of failure. As a result, the column reinforcements designed from static considerations need not be revised. 604 Structural Engineering Analysis and Design Second Edition 5.1.6.9.3 Transverse Reinforcement in Columns As mentioned, only one standard column design is adopted for both internal and external columns. Hence, the design shear force including considerations of capacity design is the more critical of the two below. (i) Exterior column : VSd,CD = γ Rd M oRd + M uRd 200.4 + 217.1 = 1.2 × = 167 kN lc 3 (i) Interior column : VSd,CD = γ Rd M oRd + M uRd 250.5 + 283.9 = 1.2 × = 213.8kN lc 3 Hence the design shear force is 213.8kN. Hoop Pattern Since the maximum distance between adjacent longitudinal bars restrained by hoop bends is 200m for ductility class ‘M’, a double hoop pattern is used. Minimum Diameter of Hoops Minimum diameter of hoops, dbw = β dbl,max (fyld / fywd) = 0.35 x 22 x (347.8/191.3) = 14.0 mm Maximum Spacing of Hoops sW = min { bc/3 ; 150mm ; 7dbl } = min { 340/3 ; 150mm ; 7x22} = 113 mm select spacing of 110 mm Confinement Coefficients αn = 1− ∑b 2 i 6A 0 = 1− 4 × 0.159 2 + 4 × 0.209 2 = 0.693 6 × 0.44 × 0.34 2 2  s  110   α S = 1 − w  = 1 −  = 0.703  2 × 340   2b 0  α = α n α S = 0.693 × 0.703 = 0.487 For ductility class ‘M’ columns, the required mechanical ratio of confinement reinforcement is: ω Wd ≥  f yd 1 k 0 µ ϕ ν d  α   ES    0.35A g / A c + 0.15 − 0.035    ω Wd ≥ 1 [60 × 9 × 0.21 × 0.00174 × (0.35 × (0.4 × 0.5) / (0.34 × 0.44) + 0.15) − 0.035] = 0.178 0.487 ( ) 605 Structural Engineering Analysis and Design Second Edition Select hoops of 10 mm diameter at spacing sw. The volumetric ratio is: ρw = (2 × 340 + 2 × 440 + 4 × 278) × 79 = 1.411 volume of hoops = volume of confined core 340 × 440 × s w sw ( ) ω Wd = ρ w f yd / f cd = 1.411 29.39 × (347.8 / 16.7 ) = sw sw ω Wd ≥ 0.178 ⇒ max imum s w = 29.39 / 0.178 = 165 mm Thus the hoop spacing is dictated by maximum spacing of hoops above. So choose φ10@110mm. Check Maximum Design Force That Can Be Carried Without Crushing of Concrete VSd = 213.8kN VRd2 = maximum design force that can be carried without crushing of concrete VRd2 = 0.5νfcdbw x 0.9d where ν = (0.7-fck/200) = 0.575 ≥ 0.5 VRd2 = 760.5 kN > 213.8kN ⇒ OK, there is no increase of dimensions required. Check If Shear Reinforcement Is Required VCD = design shear of a member without shear reinforcement VCD = [τRdk(1.2+40ρ1)+0.15σcp]bwd τRd = 0.035fck2/3 = 300kPa k = 1.6-d = 1.6-0.46 = 1.14 A 10.74 ρ= s = = 0.0061 (≤ 0.02 ) b w d 40 × 44 σ cp = 694 = 3470 kN / m 2 0.4 × 0.5 So, VCD = [300 x 1.14 x (1.2 + 40 x 0.0061) + 0.15 x 3470] x 0.4 x 0.5 =202.9 kN (<213.8 kN) Shear Resistance The shear resistance is given by the following equation; Vwd = A sw (2 + 1.45)79 × 0.9 × 0.44 × 191.3 = 187.7kN 0.9df ywd = s 110 Thus VRd = VCD + Vwd = 202.9 + 187.7 = 390.6 Outside Critical Limits The spacing of the transverse reinforcement should not exceed the lesser of the following three distances: d) 12 x the minimum diameter of the longitudinal bars = 12 x 20 = 240mm e) the least dimension of the column = 300mm f) 300mm Therefore outside the critical regions the stirrup spacing can be increased to as much as 240 mm. 606 Structural Engineering Analysis and Design Second Edition 5.1.6.10 Detailing of Beams 5.1.6.10.1 Anchorage Length The required anchorage length for bars and wires is given by: Lb,net = αa lb (As,req/As,prov) ≥ lb,min At the support; negative reinforcement anchorage length: Lb,net = 1.0 x (16/4 x (347.8/2.7)) x (14.07/13.0) = 557.7 mm At the span; Positive reinforcement anchorage length: Lb,net = 1.0 x (14/4 x (347.8/2.7)) x (9.24/8.34) = 499.5 mm 5.1.6.10.2 Curtailment of Support Reinforcement 607 Structural Engineering Analysis and Design Second Edition 5.1.7 Steel Design to EC8 for Earthquake Effects Based on Response Spectrum Analysis Sufficient local ductility of members or parts of members in compression should be ensured by restricting the width-thickness ratio b/t according to the cross sectional classes as follows. Capacity design methodology must be employed. Connections in dissipative zones should have sufficient over-strength to allow for yielding of the connected parts. Connections of dissipative parts made by means of butt welds or full penetration welds are deemed to satisfy the overstrength criterion. For fillet weld connections or bolted connections, the resistance of the connection must be factored 1.2 times the plastic moment capacity of the connected part. For bolted shear connections bearing failure should precede shear failure. Moment resisting frames shall be designed so that plastic hinges form in the beams and not in the columns. This requirement is waived at the base of the frame, at the top floor of multistorey buildings and for one storey buildings. The beam to column joints shall have adequate overstrength to allow the plastic hinges to be formed in the beams. Concentric braced frames shall be designed, so that yielding of the diagonals in tension will take place before yielding or buckling of the beams or columns and before failure of the connections. Eccentric braced frames shall be designed so that beams are able to dissipate energy by the formation of plastic bending and/or plastic shear mechanisms. The rules are intended to ensure that yielding in the plastic hinges or shear panels of the beams will take place prior to any yielding or failure elsewhere. 608 Structural Engineering Analysis and Design Second Edition 5.1.8 Timber Design to EC8 for Earthquake Effects Based on Response Spectrum Analysis 609 Structural Engineering Analysis and Design Second Edition 5.1.9 Masonry Design to EC8 for Earthquake Effects Based on Response Spectrum Analysis 610 Structural Engineering Analysis and Design Second Edition 5.1.10 Performance Based Seismic Analysis and Design Recent damaging earthquakes in the United States (1989 Loma Prieta, 1994 Northridge) and abroad (1995 Kobe, Japan; 1999 Izmit, Turkey; and 1999 Chi-Chi, Taiwan) have led the public-at-large, public officials (local, state, and federal), and owners of structures (buildings, bridges, and infrastructure) to question the utility of modern seismic design codes. Many have argued that a higher level of public safety is required (despite the extremely low likelihood that an individual will die as a result of earthquake shaking). Partially in response to the damage wreaked by the Loma Prieta and Northridge earthquakes, the United States Federal Emergency Management Agency funded studies on performance based earthquake engineering: studies that resulted in FEMA 283 (Moehle and Whittaker, Eds), FEMA 273 and FEMA 274: two documents that have been replaced by FEMA 356. When we talk about performance based seismic design, the definition of limit states for seismic design becomes extremely fundamental. They are defined as follows. I. Level I Earthquake − Serviceability Limit State (Stiffness) This limit state is so that cracking of concrete and limited steel yield due to small frequent earthquakes does not disrupt the function of the structure. Stiffness governs the response of structures in low loads because strength yet to be reached. Most operations and functions can resume immediately. Repair is required to restore some non-essential services. Damage is light. Structure is safe for immediate occupancy. Essential operations are protected. II. Level II Earthquake − Damage Control Limit State (Strength and Distribution of Strength) This limit state is so that the damage inflicted on the structure in the form of wide cracks in concrete and cover spalling and small permanent deformations in steel members due to the design earthquake is repairable. Strength and its distribution govern the response as elastic limit reached. Damage is moderate. Selected building systems, features or contents may be protected from damage. Life safety is generally protected. Structure is damaged but remains stable. Falling hazards remain secure. Repair possible. III. Level III Earthquake − Survival Limit State (Ductility) This limit state is so that the collapse of the structure and loss of life is avoided although heavy irreparable damage may occur due to the maximum credible earthquake. Ductility governs the response. Structural collapse is prevented. Nonstructural elements may fall. Repair generally not possible. Performance based seismic analysis can be performed using the multi-modal response spectrum (with no behaviour factor) methodology, random response analysis or deterministic transient analysis. 611 Structural Engineering Analysis and Design Second Edition 5.2 5.2.1 GL, ML Human Footfall Induced Vibrations 12 Limitations The proposed method does not address the analysis of very lightweight floors (e.g. domestic timber floors) where the interaction between the person walking on the floor and the floor itself is more complex, and cannot be treated simply as an applied dynamic load. 5.2.2 Finite Element Mesh and Model Parameters As with any dynamic response problem, if only the first few resonance frequencies and mode shapes are required, then a relatively coarse mesh can be used. If higher frequencies are required, then the mesh must be suitably fine to model the more complicated mode shapes. A good parameter may be the modal mass. We know that the modal mass of all the bending modes of a beam (single spanning slab) is half the total beam (single spanning slab) mass if simply supported, of a beam is quarter the beam mass if a cantilever, and of a plate is quarter the plate mass if simply supported. Refer to section 4.1.3.4 for a full explanation of natural frequency and modal mass estimation. When higher modes deviate from the correct modal mass value, then we know that the mesh cannot capture the mode shape. With more complicated structures, an h- or p-refinement should be performed and the modal masses of the original and the refined mesh should be compared; modal masses of higher modes which begin to show discrepancies indicates the extent of the capability of the mesh in capturing these higher modes. The following modal analyses of a simply supported 10m UB457x191x98 lumped mass beam model were performed in OASYS/GSA 8.0.15. We shall describe only the bending modes (not axial). The total mass of the structure is 981.3kg, hence the correct modal mass is 490.65kg. It is usually recommended that there be 4 elements (or 2n, n integer) for each half sine of mode. As the number of elements in the odd number models increases, gradually, the modal mass becomes more accurate. Beam Mesh 2 Elements 3 Elements 4 Elements 5 Elements 6 Elements 7 Elements 8 Elements Natural Frequencies (Hz) 15.03 15.14, 55.87 15.16, 57.52, 113.3 15.17, 58.19, 119.9, 179.4 15.17, 58.38, 122.2, 192.7, 249.5 15.17, 58.48, 123.3, 198.5, 269.7, 320.9 15.17, 58.53, 123.9, 201.6, 280.2, 347.3, 392.6 Modal Mass (kg) 490.6 All 654.2 All 490.6 All 542.4 490.6, 654.2, 490.6, 654.2, 490.6 All 516.2 All 490.6 Comment Very poor Good for first mode Very Poor Very Poor Poor Good for first 2 modes With floor problems, because of the high repetition of the structure, there is likelihood that there will be many modes of similar frequency. Symmetry boundary conditions may be argued, but they will only capture odd bending modes. Antisymmetric boundary conditions are required for even modes. Combination is quite impractical in dynamic response studies. Moreover, the symmetric or antisymmetric boundary conditions only capture the stiffness of the omitted structure and the correct natural frequencies. However, for response calculations, the omitted structure will result in lower modal masses if nothing else is done, and hence a higher response. Hence, the mass associated with the truncated portion of the modes have to be lumped onto the boundary to bring the modal mass up to that of the original model and hence produce the correct response. Because of these unnecessary complications, a full model is strongly recommended for dynamic analyses. 12 WILLFORD, Michael & YOUNG, Peter. Towards A Consistent Approach of Predicting Footfall-Induced Structural Vibrations. Advanced Technology Ove Arup & Partners International Ltd., London. 612 Structural Engineering Analysis and Design Second Edition Composite floors of concrete slab and steel beams if acting compositely (i.e. has sufficient shear studs for full composite action) can be modeled with shells for the slab and compatible beam elements for the beams. Offset elements should be used to model the offset between the elastic neutral axes of the slab and the beams. In these cases of composite floors, the shell formulation must include in-plane stiffness (on top of bending stiffness). If the floor has a layer of screed and/or stone finish on top of the concrete slab, the mass and stiffness should be included and the offset from the elastic neutral axes of the slab + finishing to that of the beam should be used. Connections between elements should be at their neutral axis. Connections of slabs with offset beams are no different, the elastic neutral axis should be found and both the beams and the slabs should be offset from their common neutral axis to connect into column (beam) elements. This is important especially so in linear dynamic problems where an incorrect connection point will result in incorrect mode shapes. The recommended dynamic parameters for steel and concrete are as follows. Material NW concrete LW concrete Steel Density (tonnes/m3) 2.40 1.88 7.84 Young’s Modulus (kN/m2) 38 x 106 22 x 106 205 x 106 Poisson’s Ratio 0.2 0.2 0.3 The calculation of reinforced concrete section properties can often assume the concrete is uncracked, but the nominal extreme fibre stresses should be estimated under in-service loads to validate this assumption. Normally the effect of cracking will be negligible if extreme fibre stresses are less than 2N/mm². The objective is to obtain the best estimate of the natural frequency, and when cracking is extensive, judgment is required to assess the most representative section properties to assume. The section properties so derived should be based on dynamic E values and allow for tension zone stiffening. If it is expected that the concrete may be cracked then a reduced Young’s modulus should be used. Concrete screeds, when they are present, can be included as contributing to dynamic stiffness. At the very low strain levels associated with footfall vibration it can usually be assumed that structural elements are fully continuous and behave in a fully composite manner unless connections are detailed specifically to prevent this (e.g. true pin connection, truss supported at top chord only). Normally for strength or serviceability design structural engineers will assume pinned end connections. For dynamics assume all connections are fixed unless they truly are pins. This is due to the very small strains involved with dynamics. An external wall or façade can generally be assumed to offer a continuous line of support to the floor edge. If you have a façade around your building it may offer vertical support to your floor. Due to the small strains involved with dynamics provide vertical restraint at façade locations. The same applies around concrete core walls. Columns offer rotational stiffness to floor beams assuming full continuity as well as vertical support. If modelling a floor plate with pin supports at column positions the rotational stiffness of the beams can be increased by removing the pin supports and modelling the columns above and below the floor. The bending stiffness of the columns will help increase the natural frequency of the floor. There is also the danger of over restraining. If modelling a floor plate using 2D elements and offset beams, make sure that the slab edges are not fully restrained against moving laterally (i.e. that it is pinned). Otherwise, this will result in the slab attracting membrane forces and will give a higher natural frequency than the floor actually has. The best estimate of the in-service mass should be used. The actual mass of fit-out in a building is often significantly less than the design allowances, and actual live loads in offices are often only 10% of the design value, and are negligible on footbridges. Typically the non-structural mass for an office floor can be taken as 100kg/m2. Do NOT apply the full live load as added mass. For stairs and bridges NO live load should be added. It should be noted that over-estimating the mass can often result in unconservative predictions of dynamic response. For trapezoidal decking, you may need to modify the density of the 2D elements to take account of the large voids in trapezoidal decking. It is vital that mass is correctly modeled to calculate the right natural frequencies and modal masses. 613 Structural Engineering Analysis and Design Second Edition Damping values quoted in the literature for floors have often been estimated from heel-drop tests and caution must be used with these values. The damping so obtained is usually not a true measure of modal damping because several modes are responding together, and the initial decay of a heel drop includes transfer of energy between modes as well as dissipation. The apparent damping so obtained is too high. It has been seen that for composite structures the effective damping tends to decrease as the span increases. This may be due to the greater size of the steel elements (which have lower intrinsic damping than concrete) relative to the concrete in longer spans. For a typical composite office floor or reinforced concrete floor with partitions and raised floors damping of 3% of critical may be assumed. For a composite floor with no furniture, partitions, raised floors (e.g. airport terminal) damping may be as low as 1.0% of critical damping. 614 Structural Engineering Analysis and Design Second Edition 5.2.3 (Non-Crowd or Asynchronous) Human Induced Vertical Footfall Vibrations from Walking This is evaluated for a single person walking. If several people are walking together, unless they are marching in a disciplined manner, the footfall rates and phasing will not be coordinated, and hence the response will not increase in proportion to the number of people. The response due to a single person walking is most when the structure is empty as to minimize the modal mass and not add additional human damping. It has been observed that the damping of a structure increases if a large number of people are present on the structure. The human body can be represented as a dynamic system having two or more main degrees of freedom. 5.2.3.1 Dynamic Response To Vertical Dynamic Forces From Walking on Flat and on Stairs Depending on the relative frequencies of harmonic excitation and the natural frequencies of the structure, a different response will be obtained. The following graph shows a 2Hz and a 26Hz floor being excited by 2Hz walking. There is clear resonant build-up in the first case and clear individual transient response in the second case. Response Transient and Resonant Responses 0 0.5 1 1.5 2 2.5 3 3.5 4 4.5 5 Time 5.2.3.1.1 Resonant Excitations For Modes Up To 15Hz (Flat) and 22Hz (Stairs) In this LINEAR FREQUENCY DOMAIN solution, not only that the static response has to be added separately, but also the mean of the dynamic excitation has also got to be added separately as a static response. This is because the mean of the dynamically applied force is not included in the dynamic excitations. Hence the total response in this frequency domain dynamic analysis = static response to mean of dynamic excitation + dynamic response + static response to static loads. However, usually in footfall induced response, it is not the total response which is of importance, as the criteria is not from a structural safety viewpoint, but rather from a human comfort viewpoint, the latter of which is measured in terms of acceleration and velocity. Hence, it is sufficient to consider the fluctuations of the dynamic response. The static response to the mean of the dynamic excitation can be ignored. Typical single and continuous footfall force time histories are presented. These are inharmonic periodic signals. 615 Structural Engineering Analysis and Design Second Edition The first graph shows the Load/(Static Weight) to be greater or less than 1.0, which represents the static weight. Taking the mean as the static weight, the dynamic load excitation can then be defined with positive and negative fluctuations as shown on the second graph. It can be seen that the ‘positive’ downward force phase is generally shorter and of higher magnitude than the negative force phase. Note that the positive and negative here are relative to the static weight of the person. These time histories can be decomposed into their frequency components by Fourier Series analysis. The amplitude of the frequency component time histories relative to the static load is called the dynamic load factor, clearly less than 1.0 because these are the amplitude of the fluctuations about the mean static weight. The dynamic load factor (not the (magnitude of the) dynamic amplification factor) multiplied by the static load is hence the amplitude of the dynamic excitation, for a particular harmonic frequency component. EC5 BS5400 Bear in mind that the total response will then be that of the dynamic response plus the mean of the dynamic excitations, i.e. the static weight of the person, plus the static response due to the static loads on the structure. As always done in frequency domain analyses, the mean is applied separately to the dynamic fluctuations. However, in the case of floor excitations, we are usually only interested in the dynamic acceleration or velocity response and not the total (static + dynamic) displacement response. These curves show that the footfall time histories can be decomposed into 4 harmonic components. The Arup DLF curves for walking on flat (floors and footbridges) are reproduced for clarity. Dynamic Load Factor For Walking on Flat The DLFs are the magnitudes of the sinusoidal harmonic components (for frequencies at 1, 2, 3 … etc … of the walking frequency) derived by Fourier Analysis, that when added together, will recreate the original force time history. 0.60 0.50 DLF 0.40 0.30 0.20 0.10 0.00 0 2 4 6 8 10 12 Forcing Frequency (Hz) Harmonic 1 Harmonic 2 Harmonic 3 Harmonic 4 616 Structural Engineering Analysis and Design Second Edition The Arup DLF curves for walking on stairs are also presented. Note that the DLFs for walking on stairs are greater than for walking on flats. Also, the frequency range is higher, i.e. first harmonic frequency range is up to 4.5Hz for walking on stairs compared to 2.8Hz for walking in flats. Dynamic Load Factor For Walking on Stairs 1.20 1.00 DLF 0.80 0.60 0.40 0.20 0.00 0 5 10 15 20 Forcing Frequency (Hz) Harmonic 1 Harmonic 2 Harmonic 3 Harmonic 4 Multi-Modal Response Analysis It is the practice to perform resonant response calculations for single person walking excitations, albeit at the most critical footfall rate, not necessarily the highest or the lowest footfall rate, but usually that which corresponds to the natural frequency of the structure. We say usually because the DLF varies. For instance, if we had a stair of fundamental frequency 2.0Hz, we need to consider the response due to excitation at 2.0Hz to maximize the dynamic amplification (but at a lower DLF) and also the response at 2.7Hz to consider the maximum DLF, but offresonant response, but yet as close to 2.0Hz with maximum DLF. If several people are walking together, unless they are marching in a disciplined manner, the footfall rates and phasing will not be coordinated, and hence the response will not increase in proportion to the number of people. The first harmonic component varies from frequencies of 1Hz to 2.8Hz for walking on flats and from 1Hz to 4.5Hz for walking on stairs. The DLF versus harmonic excitation frequency curves are very illustrative. Since resonant vibrations response is far more significant than impulsive response in any field of dynamic excitation, we would ideally like to avoid any form of resonance. For footfall vibrations, resonance with the first harmonic is clearly most damaging since the DLF associated with the first harmonic is the largest. Hence if the fundamental vertical natural frequency of the structure is significantly more than 2.8Hz or 4.5Hz (whichever relevant), the resonance with the first harmonic is avoided. Similarly, if fundamental vertical natural frequency of the structure is significantly more than 5.6Hz or 9.0Hz (whichever relevant), the resonance with the second harmonic is avoided. Finally, if fundamental vertical natural frequency of the structure is significantly more than 8.4Hz or 13.5Hz (whichever relevant), the resonance with the third harmonic is avoided, although to obtain resonance with the 3rd 617 Structural Engineering Analysis and Design Second Edition (or 4th for that matter) harmonic is quite difficult anyway. It should be noted that FOR STAIRS resonance of the second harmonic has been observed but NOT of the third and higher harmonics, probably because of imprecise loading. If we were to consider resonance of modes due to 4th harmonic excitations, we would need to consider modes up to 11.2Hz and 18.0Hz (for walking on flat and stairs respectively). Let us then solve for modes up to say 15Hz and 22Hz (flat and stair respectively) to also capture the off-resonant responses of modes higher then 11.2Hz and 18.0Hz. The calculation procedure is now illustrated. A conventional modal frequency domain analysis is performed. The equation of motion in the time domain is [M ]{& u&( t )} + [C]{u&( t )} + [K ]{u ( t )} = {P( t )} In the frequency domain we let {u(t)} = Re al [[Φ ]{ξ(ω)}eiωt ] where {ξ(ω)}is a complex modal displacement response function vector {P(t)} = Re al [{P(ω)}e iωt ] where {P(ω)}is a harmonic loading function vector And orthogonalizing the coupled equations, leads to a set of uncoupled equations in the form for a mode i −ω 2 M i ξ i (ω) + iCi ωξ i (ω) + K i ξ i (ω) = Pi (ω) Rearranging for the complex modal response (in modal space) ξ i (ω) = p 0i − ω M i + iC i ω + K i = p 0i − ω 2 M i + K i + iC i ω = (1 − ω 2 p 0i / K i 2 ) / ω ni + i(2ζ i ω / ω ni ) 2 Instead of the polar form, this can be written in terms of the real and imaginary parts ( ) 2  p 0i  (2ζ i ω / ω ni ) 1 − ω 2 / ω ni   − i 2 2 2  2 K i  1 − ω 2 / ω 2 2 + (2ζ ω / ω )2 1 − ω / ω + ( 2 ζ ω / ω ) ni i ni ni i ni   ξ i (ω) = ξ iREAL (ω) − iξ iIMAG (ω) ξ i (ω) = ( ) ( ) Thus, the steady-state solution in the time domain {u ( t )} = Re al [[Φ ]{ξ REAL (ω) − iξ IMAG (ω)}e iωt ] {u ( t )} = Re al [[Φ ]{ξ REAL (ω) − iξ IMAG (ω)}(cosωt + isinωt )] {u ( t )} = [Φ ]{{ξ REAL (ω)}cos ωt + {ξ IMAG (ω)}sin ωt} Note that this expression is to be interpreted as {u ( t )} = [{φ}1 ... {φ}i  p 01   K (D1REAL (ω) cos ωt + D1IMAG (ω) sin ωt )   1  ...   p  ... {φ}n ] 0i (D iREAL (ω) cos ωt + D iIMAG (ω) sin ωt )  K  i  ...    p 0n (D  nREAL (ω) cos ωt + D nIMAG (ω) sin ωt ) K  n  618 Structural Engineering Analysis and Design Second Edition where D iREAL (ω) = D iIMAG (ω) = (1 − ω / ω ) / ω ) + (2ζ ω / ω 2 2 (1 − ω ni 2 2 2 ni i ni )2 (2ζ i ω / ω ni ) (1 − ω2 / ωni 2 )2 + (2ζ i ω / ωni )2 Since MAX (Acosωt + Bsinωt) = (A2+B2)½, at a particular DOF j, the steady state displacement response will be  Steady − State Response, u jMAX =   n ∑ i 2   p 0i φ ij D iREAL (ω)  +  Ki   n ∑ i  p 0i φ ij D iIMAG (ω)  Ki  2 The expression for acceleration can be obtained simply by differentiating the displacement expression twice w.r.t. time. Hence there will be a multiple of the square of the excitation frequency, ω2. The above expression is exact for excitations at a certain point long enough for steady-state conditions to be achieved. In practice of course, the number of footfalls are limited (a pedestrian is only effective in generating resonant response when walking along a single half sine wave of the mode shape; as he moves on to the next, out of phase half sine wave he begins to cancel out the vibration he has just generated) and not all these footfalls are applied at the same mode-shape point (many of the steps will have been towards the edge or the less active part of the half sine and would have been less effective in generating response). Hence, only a proportion of the maximum possible steady-state is the achieved. The maximum proportion of steady-state response for crossing a sinusoidal mode shape can be estimated as where N is approximately 0.55 of the total number of vibration cycles occurring as the span is crossed. The total number of cycles for first harmonic loading is the span distance L divided by the stride length l, and for higher harmonics this number of cycles is multiplied by the harmonic number n. This expression for r is best applied ONLY to the imaginary parts in this procedure. It is also noted that the harmonic components of the footfall forcing function are not in phase. The actual phases of these harmonic components vary considerably between different persons and walking speeds. There is therefore no general relationship of phases that can be used to generate a unique time history. Hence it is recommended that the maximum response amplitude be estimated by means of the SRSS combination of the individual responses of each harmonic. The peak acceleration can be compared to peak acceleration acceptability criteria in the 1/3 octave bands. Alternatively, the RMS acceleration response is derived from the maximum response (by dividing by √2 since simple harmonic motion) and comparison to the RMS acceptability criteria in the 1/3 octave bands is made. Let us illustrate the resonant response calculation for ALL modes exactly for the response at ONE node due to excitation at ONE harmonic frequency, say 5.14Hz (corresponding to the second harmonic of a walking frequency of 2.57Hz). This harmonic frequency corresponds to the first mode. Hence the first mode resonates whilst the rest of the modes present off-resonant response. Mode Natural Frequency, fn (Hz) Excitation Frequency, f (Hz) f/fn Modal Damping DiREAL DiIMAG 1 5.14 5.14 1.00 0.03 0.000 16.667 2 5.39 5.14 0.95 0.03 7.890 4.982 3 6.30 5.14 0.82 0.03 2.928 0.429 4 8.28 5.14 0.62 0.03 1.621 0.098 619 Structural Engineering Analysis and Design Second Edition Say that the excitation node and response node is the same and corresponds to unity modal displacement for mode 1. The amplitude of the modal force for mode 1 is thus, p01 = 1.0 x DLF x 700N = 1.0 x 0.098 x 700 = 68.5N. φr(p0i/M). Modal Displacement at Modal Force Amplitude, Modal Displacement at φr(p0i/M). 2 2 (f/fn) .DiREAL (f/fn) .DiIMAG p0i = 68.5φe Response Node, φr Modal Mass Excitation Node, φe 29551 1.000 68.500 1.000 0.00000 0.03863 29551 0.953 65.260 0.953 0.01510 0.00953 29551 0.816 55.899 0.816 0.00301 0.00044 29551 0.621 42.552 0.621 0.00056 0.00003 0.01866 0.04864 The steady-state response is then (0.018662 + 0.048642)1/2 = 0.0521ms-2. Assuming a stride length of 0.75m the number of steps to cross the span is 16, resulting in 32 cycles of vibration at the 2nd harmonic frequency. The proportion of steady state response for 3% damping is then obtained, r = 1-e-2π0.03N = 0.96 where N = 0.55x32 = 17.6. Hence the corrected steady-state response is 0.96 x 0.0521 = 0.050ms-2. And thus the response factor, R = 0.050/0.007 = 7.1. The peak acceleration responses at A NODE due to excitation at A NODE (not necessarily but usually the same node), for ALL harmonic forcing frequencies (from walking on flat) can be presented as follows. The graph shows that the maximum response occurs due to the second harmonic at 5.2Hz. There is clearly a significant (to the response at THIS NODE) natural mode at this frequency. There are also natural modes at 6.3Hz and 7.1Hz, but the maximum response comes from the second harmonic, which has a larger DLF. Notice that the first harmonic, which has the greatest DLF, does not peak because there is no significant natural mode within the frequency range of the first harmonic. Individual Harmonic Peak Acceleration At A Node For All (Flat) Harmonic Frequencies Resonance of second harmonic excitation with natural frequency at 5.2Hz. Peak Acceleration (%g) 1.6 1.4 1.2 Harmonic 1 1.0 Harmonic 2 Harmonic 3 0.8 Harmonic 4 0.6 0.4 0.2 0.0 1 3 5 7 9 11 13 Harmonic Forcing Frequency (Hz) The response at A NODE due to excitation at A NODE can also be presented in terms of the walking frequency i.e. the frequency of the first harmonic. The former graph is more illustrative as it shows the response in terms of the individual harmonic frequencies, not just the first harmonic (i.e. walking frequency). 620 Structural Engineering Analysis and Design Second Edition Individual Harmonic Response Factor At A Node For All (Flat) Walking Frequencies Resonance of second harmonic excitation with natural frequency at 5.2Hz. 1.8 Response Factor 1.6 1.4 Harmonic 1 1.2 Harmonic 2 1.0 Harmonic 3 0.8 Harmonic 4 0.6 Total Response Factor 0.4 0.2 0.0 1 1.5 2 2.5 3 Walking Frequency (Hz) The MAXIMUM response at EACH AND EVERY NODE giving consideration to ALL the harmonics altogether can be computed and presented as follows. 621 Structural Engineering Analysis and Design Second Edition Fundamental Mode Response Analysis – Hand Calculation A single fundamental mode response usually provides good approximations to the maximum response because of the fact that different modes are out of phase with each other, their maximums at a point not occurring at the same time. Hence, for a floor plate, the maximum response in the middle of the plate is usually governed just by the fundamental mode. Higher modes have higher natural frequencies and hence the modal stiffness will be larger, resulting in a lower modal response. This approximation begins to fall apart when there are modes closely spaced, in which case the multi-modal approach should be used. The multi-modal approach should also be used if the response due to the first harmonic exciting a mode and higher harmonics exciting another mode is required. Of course, the multi-modal approach also considers multiple modes (albeit most of them contributing off-resonant response). To ascertain the most significant mode for the response to excitation at a particular node, scroll (visually or numerically) through all modes and pick out the modes with the greatest displacement value at that node. This gives the modes with the highest modal force. Of these, mode with the lowest modal mass will obviously yield the highest response. Hence, pick out the mode with the lowest modal mass (by FE computation or otherwise) or by visual inspection knowing that modes that mobilize more of the structure will be have a larger modal mass associated with it. Because we need not consider the phase information (since no mode combinations are required), we do not need to express the dynamic amplification in terms of its real and imaginary parts. Instead, we consider the magnitude of the dynamic amplification function straight away. This gives the steady-state (i.e. peak) acceleration response in physical coordinates as a peak = φ response φ excitation ω2 p0 (1 − ω ω ni M i 2 1 2 / ω ni ) 2 2 + (2ζ i ω / ω ni ) 2 And at resonance (ω = ωni), a peak = φ response φ excitation p0 1 M i 2ζ i Inculcating the proportion of steady-state response achievable for crossing span a peak = φ response φ excitation r p0 1 M i 2ζ i where r = 1 − e −2 πζN , N = 0.55n L λ For the maximum (peak) response with excitation at the maximum point of the mode shape and the weight of a person as 70kg (about 700N), a peak = (1.0)(1.0)r 700 x DLF 1 Mi 2ζ i where r = 1 − e −2 πζN , N = 0.55n L λ where the DLF corresponds to the excitation frequency equal (as resonance response intended) to the natural frequency of the mode under consideration. The peak acceleration can be compared to peak acceleration acceptability criteria in the 1/3 octave bands. Alternatively, the RMS acceleration response is derived from the maximum response (by dividing by √2 since simple harmonic motion) and comparison to the RMS acceptability criteria in the 1/3 octave bands is made. Hence, if the excitation is between 4Hz < fharmonic excitation < 8Hz, then Re sponse Factor = a peak 0.007 or Re sponse Factor = 622 a RMS a peak / 2 a peak = = 0.005 0.005 0.007 Structural Engineering Analysis and Design Second Edition 5.2.3.1.2 Transient Excitations For Modes Above 15Hz (Flat) and 22Hz (Stairs) In this LINEAR TIME DOMAIN solution, the static response must be added to the dynamic response if the dynamic analysis is performed about the initial undeflected (by the static loads) state with only the dynamic loads applied, hence causing the dynamic response to be measured relative to the static equilibrium position. Hence, the total response = the dynamic response + the static response to static loads. Alternatively, in this LINEAR TIME DOMAIN solution, if the dynamic analysis is performed with the deflected static shape as initial input and the static loads maintained throughout the dynamic excitations, the total or absolute response (static and dynamic) is obtained straight away from the dynamic analysis. Hence total response = dynamic response (which already includes the static response to static loads). However, usually in footfall induced response, it is not the total response which is of importance, as the criteria is not from a structural safety viewpoint, but rather from a human comfort viewpoint, the latter of which is measured in terms of acceleration and velocity. Hence, it is sufficient to consider dynamic response due to the impulse excitations. This ignores the static response to static loads such as that of the floor, but does inherently include the static response to the mean of the dynamic excitation (unlike the frequency domain approach). Typical single footfall force time histories are presented. Multi-Modal Response Analysis Where resonance excitations cannot occur, the response will be governed by an impulsive type response, i.e. the starting transient response will be more significant than the steady-state response (or that during the build up of the steady-state response), giving a much lower dependency of response on the exact frequency and on damping. The calculation procedure is illustrated. The dynamic equation of motion in the time domain is [M ]{& u&( t )} + [C]{u&( t )} + [K ]{u ( t )} = {P( t )} Orthogonalizing the coupled equations, leads to a set of uncoupled equations in the form for a mode i Mi & ξ&i ( t ) + C i ξ&i ( t ) + K i ξ i ( t ) = Pi (t) for the i th mode On rearranging, the modal response in modal coordinates ξi ξ i (t ) = D i (t ) p 0i p = D i ( t ) 2 0i Ki ω ni M i Finally, the response in physical coordinates ui(t) are {u(t)} = [Φ ]{ξ( t )} 623 Structural Engineering Analysis and Design Second Edition In the case where the excitation is impulsive (t1/T < ~0.2), the maximum modal displacement response will be ξ i max = 1 M i ω ni ∫ ξ i max = 1 M i ωdi ∫ τ= t τ =0 τ= t τ =0 φ i p(τ)dτ undamped φ i p(τ)dτ damped Response formula becomes less valid for higher modes of vibration as t1/Ti > ~0.2 where φ i = mod al component at excitation point And, the displacement response in physical coordinates ui(t) are {u(t)} = [Φ ]{ξ( t )} In time domain analyses the maxima of the modal responses in physical space do not occur at the same time. Hence, the exact procedure would be to write the total response in physical space as above and only then maximize the function. If however the modal responses were to be maximized, then some sort of combination technique such as the SRSS or CQC should be employed. For impulsive excitation though, the maximum response occurs at the first cycle of ensuing vibration after impact. The phase difference between modes is quite insignificant as it takes time for damping to affect the phase between the modes. Hence the maximum response can be approximated as a simple summation of the maximum response of the individual modes. For response due to impulsive type excitations, only one footfall excitation is required as the maximum occurs at the very first cycle. The ensuing vibration is the unforced vibration of the structure at its damped natural frequencies. Hence the maximum (peak) modal velocity response is obtained (by differentiating w.r.t time) 1 τ= t ξ&i max = φ i p(τ)dτ M i τ =0 ∫ For flats, the value of the (empirical) effective impulse, Ieffective (with 25% exceedance probability) can be taken as I effective = ∫ τ= t τ= 0 φ i p(τ)dτ = φ i 54 f 1.43 Ns f n1.30 where f is the excitation frequency and fn the natural frequency. For stairs, the value of the (empirical) effective impulse, Ieffective can be taken as τ= t 150 I effective = φ i p(τ)dτ = φ i Ns τ =0 fn ∫ And, the velocity response in physical coordinates are {u&(t)} = [Φ ]{ξ&( t )} The maximum (peak) velocity response is approximated by the simple addition of the maximum individual modal velocity responses, although this is not strictly correct. With modal methods, the quantity for every mode (be it the displacement, velocity, acceleration, stress or force) must be combined before being maximized. Note that you can derive the velocity and acceleration for every mode to be combined, and not just the displacement. But the fact remains that the maximizing must be performed after modal combination. But because we are assuming that all modes are responding in an impulsive nature (although clearly this assumption is NOT TRUE for higher modes of vibration) we shall maximize the response of individual modes before combination, because we are assuming that the phase difference between modes to be insignificant for the reason outlined above (that all modes response in an impulsive nature) and that damping is not prominent to affect the phase in the first cycle. Alternatively, the correct method of modal combination should be used. Here the different modal responses in the physical coordinates are combined before maximizing the function, which is as follows. 624 Structural Engineering Analysis and Design Second Edition u&( t ) = N ∑ φ ξ&e i i − ζ i ωni t sin ω di t i =1 The peak velocity CANNOT be compared to peak velocity acceptability criteria because the response is characterized by a series of decaying transient vibrations and hence the peak velocity is unrepresentative in perceptibility terms. An effective peak value of √2 times the RMQ velocity response in the 1/3 octave bands can be used in comparison to the peak velocity acceptability in the 1/3 octave bands. Alternatively, the RMS or RMQ velocity response in the 1/3 octave bands can be compared to the RMS or RMQ velocity acceptability criteria in the 1/3 octave bands. Fundamental Mode Response Analysis – Hand Calculation For a fundamental mode response analyses, the maximum (peak) velocity response is given by I v peak = φ response effective Mi For flats, the value of the (empirical) effective impulse, Ieffective (with 25% exceedance probability) can be taken as I effective = ∫ τ= t τ =0 φ i p(τ)dτ = φ excitation 54 f 1.43 Ns f n1.30 where f is the excitation frequency and fn the natural frequency. For stairs, the value of the (empirical) effective impulse, Ieffective can be taken as I effective = ∫ τ= t τ =0 φ i p(τ)dτ = φ excitation 150 Ns fn The peak velocity CANNOT be compared to peak velocity acceptability criteria because the response is characterized by a series of decaying transient vibrations and hence the peak velocity is unrepresentative in perceptibility terms. An effective peak value of √2 times the RMQ velocity response in the 1/3 octave bands can be used in comparison to the peak velocity acceptability in the 1/3 octave bands. Alternatively, the RMS or RMQ velocity response in the 1/3 octave bands can be compared to the RMS or RMQ velocity acceptability criteria in the 1/3 octave bands. The approximate equivalent RMS velocity response is 2 v peak v RMS = 3 2 Hence, if the excitation is fharmonic excitation > 8Hz, then v a 2πfv RMS Re sponse Factor = RMS or Re sponse Factor = RMS = 0.0001 ~ 0.005 ~ 0.005 Expanding the former expression, v 1 2 v peak Re sponse Factor = RMS = ≈ 4700 v peak 0.0001 0.0001 3 2 625 Structural Engineering Analysis and Design Second Edition 5.2.3.2 Serviceability Acceptance Criteria The perceptibility and then acceptance criteria can be established in terms of peak, RMS or RMQ of a signal. RMQ has been shown to be the most reliable parameter. BS6472:1994 states the threshold of human perception in terms of the baseline RMS vertical acceleration versus vibration frequency. BS5400 70 EC5 Bachmann 20 7 proportional to velocity 1 proportional to acceleration Between 4 and 8Hz, the baseline RMS acceleration is 0.005ms-2 corresponding to a baseline peak acceleration (for steady state signals) of 0.007ms-2. The rising acceleration criteria for frequencies above 8Hz correspond to a constant RMS velocity of 0.0001ms-1. The so-called Response Factor is the number of multiples the response acceleration or velocity is that of this baseline. Structure Hospital Floor Special Office Floor Normal Office Floor Busy Office Floor Heavy Public Stairs Light Office Stairs Very Light Escape Stairs External Footbridge Acceptable Response Factor 1 4 8 12 24 32 64 50+ Increasingly over the last thirty years vibration-sensitive equipment has been used within research laboratories and production facilities in the fields of microelectronics, opto-electronics, metrology, biotechnology and medicine. Vibration levels far below human perception thresholds are normally required for these facilities, because vibration at the equipment support points can cause internal components, study specimens, or items being produced, to move relative to each other. Therefore, these facilities call for close attention to vibrations, particularly on suspended floor structures. For example, a typical semiconductor production facility might have for its 5,000m2 clean room a 1m deep concrete grillage floor supported on columns spaced at 4m x 4m. A medical laboratory floor, which might 626 Structural Engineering Analysis and Design Second Edition have vibration requirements an order of magnitude less stringent, might be designed with conventional slab/deck/steel-framing schemes similar to, but significantly stiffer and heavier than conventional office building framing. General vibration criteria as measured in one-third octave bands of frequency over the frequency range 8 to 100 Hz for laboratories are as follows. 627 Structural Engineering Analysis and Design Second Edition 5.2.3.3 Practical Solutions Flats or stairs that have fundamental frequency falling near that of the first harmonic are completely unsuitable for service. With stairs, if the stiffness of the stringers can be increased by having deeper beam sections or by tying the stringers together, then the natural frequencies of the stair would increase, hence making it less susceptible to human induced footfall vibrations. Another solution would be to have greater mass by incorporating heavier treads or by using glass along the hand railings, hence reducing the modal response, although of course the natural frequencies may decrease too much as to make it again susceptible to footfall excitation frequencies. Alterations to the boundary conditions can also be recommended at times to increase the natural frequencies of the stair, for instance by making the extremities of the stair encastre or if possible by breaking the span with a column, a beam or a hanger. As a last resort, a TMD would have to be designed and installed if all other solutions prove unacceptable to the architects. On floor vibration problems, the uniformity of the floor between adjacent bays will help lower the response. This is because the more uniform the bays are, the greater the contribution of the mass from adjacent bays into the modal mass of a particular mode. Of course, the higher the modal mass of a particular mode, the smaller will be the response. To illustrate this, consider two adjacent bays, one much stiffer than the other, here by virtue of the shorter length. Clearly, because of the small components of the eigenvector in the stiff bay, its contribution to the modal mass will be minimal. On the other hand, if the bays were of similar stiffness, the eigenvector will be more uniform and there will be a greater contribution to the modal mass from both bays. 1.0 1.0 1.0 Another case is bays that are adjacent to holes or isolated bays. The modal mass is provided by the mass only in that bay. No contribution from adjacent bays. The modal mass is thus low and the mode becomes a local mode. This is akin to a bridge really. Thus, the response can be high. Stiffness, mass and damping are the three parameters that the designer can vary to improve the dynamic performance of a floor when the basic geometry has been fixed. The true implications of making changes can only be assessed if there is proper understanding that it is a dynamic problem under consideration, with acceleration (not deflection) usually the quantity of concern. The way in which footfall force vary with frequency must also be properly appreciated. Whilst there is a decrease in footfall forces as the harmonic number increases, there is also an increase in footfall force with increasing walking speed within each harmonic, especially for the first harmonic. It is not therefore always advantageous to increase the natural frequency of a floor to reduce accelerations. Unless increasing the natural frequency takes it out of the range of susceptibility to a particular harmonic, the increase in frequency may be counter-productive. There is a strong case for saying that a floor of 3.0 to 3.6Hz natural frequency has a lower likelihood of excessive vibration than one of 3.6 to 4.4Hz. Both ranges are susceptible to the 2nd harmonic of footfall forces, but the forces are lower for the lower walking speeds that would excite the lower frequency range. Increasing the damping is always beneficial, but cannot currently be done inexpensively. Increasing the mass is also always beneficial, unless by so doing the natural frequency is reduced below a threshold that makes the floor susceptible to a lower harmonic of footfall force. Increasing the stiffness is not always beneficial; as noted above, increasing the natural frequency can render a floor susceptible to higher footfall forces from faster walking rates. Additional stiffness which takes the natural frequency above one of the thresholds is however beneficial. Experience has shown that if responses as high as R=8 are measured in offices there is occasional adverse comment, particularly if these levels are reached regularly, and lower targets (R=4-6) are recommended as necessary to remove the likelihood of such comment. 628 Structural Engineering Analysis and Design Second Edition 5.2.4 (Non-Crowd or Asynchronous) Human Induced Vertical Footfall Vibrations from Sports in Halls 13 In this LINEAR FREQUENCY DOMAIN solution, not only that the static response has to be added separately, but also the mean of the dynamic excitation has also got to be added separately as a static response. This is because the mean of the dynamically applied force is not included in the dynamic excitations. Hence the total response in this frequency domain dynamic analysis = static response to mean of dynamic excitation + dynamic response + static response to static loads. However, usually in footfall induced response, it is not the total response which is of importance, as the criteria is not from a structural safety viewpoint, but rather from a human comfort viewpoint, the latter of which is measured in terms of acceleration and velocity. Hence, it is sufficient to consider the fluctuations of the dynamic response. The established dynamic response calculation theories for walking on flats and stairs are generally equally applicable to predicting (single person) induced vibrations due to sports in halls. Certain terms such as the maximum proportion of steady-state response for crossing a sinusoidal mode shape where N is approximately 0.55 of the total number of vibration cycles occurring as the span is crossed may or may not be applicable as the excitation may be assumed located at the same spot, as the critical consideration. The DLFs for the different activities are presented as follows according to Bachmann. Activity Running Jumping Activity Rate (Hz) 2.0Hz to 3.0Hz Normal 2.0Hz Normal 3.0Hz High 2.0Hz High 3.0Hz Standing 0.6Hz 1st Harmonic DLF 1.6 1.8 1.7 1.9 1.8 DLF½ = 0.5 2nd Harmonic DLF 0.7 1.3 1.1 1.6 1.3 3rd Harmonic DLF 0.2 0.7 0.5 1.1 0.8 For a single mode, the maximum (peak) resonant response with excitation at the maximum point of the mode shape and the weight of a person as 70kg (about 700N), the peak acceleration is a peak = (1.0)(1.0) 700 x DLF 1 Mi 2ζ i where the DLF corresponds to the excitation frequency equal (as resonance response intended) to the natural frequency of the mode under consideration. If the excitation is between 4Hz < fharmonic excitation < 8Hz, then a peak Re sponse Factor = 0.007 Peak acceleration criteria is normally in the range of 0.05g to 0.1g. However, lower values may be required for adjacent floor areas housing different quieter occupancies to which vibration may be transmitted. 13 BACHMANN, Hugo. Vibration Problems in Structures Practical Guidelines. Birkhauser, Berlin, 1995. 629 Structural Engineering Analysis and Design Second Edition 5.2.5 Crowd Induced (Synchronous) Vertical Footfall Vibrations for Gymnasium Floors, Dance Floors, Stadium Tiers, Theatre Tiers and Balconies 14 This concerns excessive vibrations caused by groups of people dancing or jumping in unison. The vibrations may cause excessive motion resulting in panic, failure of non-structural components or in the most severe case, low cycle fatigue failure. We shall focus on whole body jumping since this result in the highest loadings and will be critical for most designs. Unlike the single person walking or running excitation, crowd induced vibrations differ in the sense that the loading is applied at the same location and also in the fact that the excitation is applied over a large spatial area simultaneously, i.e. crowd loading and not single human footfall loading. In this LINEAR FREQUENCY DOMAIN solution, not only that the static response has to be added separately, but also the mean of the dynamic excitation has also got to be added separately as a static response. This is because the mean of the dynamically applied force is not included in the dynamic excitations. Hence the total response in this frequency domain dynamic analysis = static response to mean of dynamic excitation + dynamic response + static response to static loads. Clearly only the fluctuations of the dynamic excitation is required to predict the response accelerations and velocity to meet the human comfort criteria, but when an evaluation of the structural integrity is required, the dynamic response must be supplemented by the mean of the dynamic excitations, i.e. the static weight of the people, and also the static response due to the static loads on the structure. If the natural frequency of a structure is significantly above the frequency at which repeated dynamic forces can be applied, then excessive vibration is unlikely to arise. Therefore the simplest form of check on the adequacy of a structure is to ensure that its natural frequencies are higher than the maximum frequency of effective excitation. If a minimum natural frequency of the structure is above the target value, then no further check is required. If natural frequencies are below the minimum target value, then the actual response of the structure has to be estimated; this is a more detailed and uncertain calculation. BS6399 Part 1: 1996 requires the dynamic response of structures with natural frequencies below 8.4Hz in the vertical direction and 4.0Hz in the horizontal direction to be considered explicitly. For stands occupied during pop concerts, the suggested minimum vertical frequency is intended to ensure that the second harmonic of jumping excitation is out of the frequency range. The following values are proposed in the literature. IStructE Guide 6.0Hz Bachmann and Ammann 7.5Hz CEB 6.5 – 7.5Hz NBCC (varies with mass of structure) 6.5Hz (typical) There is also the question of whether the natural frequency should be calculated with the mass of the audience on the stand. The IStructE Guide suggests the unloaded frequency can be used but the NBCC suggests the weight of participants should be included. Ellis and Ji have observed that the mass of stationary people should be included, but that members of the audience engaged in jumping provide dynamic force only and do not contribute mass that would lead to a reduction in frequency. There is very little guidance in the literature for swaying. Isolated measurements indicate that typical frequencies lie below 1.5Hz. International guidance of Bachmann and CEB suggest lateral frequencies should be above 2.5Hz; however, for a large crowd we assume that the effect of the second harmonic is negligible, and the minimum natural frequency should be above 1.5Hz. The IStructE does not specify a minimum natural frequency, but requires the strength of the stand to be checked for a lateral load of 7.5% of the weight of the audience, with appropriate imposed partial load factor. In a very large crowd, some reduction of DLF is expected, particularly in the higher harmonics. In addition, it becomes difficult for a large crowd to synchronize at jumping frequencies above 2.8Hz and the National Building Code of Canada suggests that the highest jumping rate to be considered is 2.75Hz. A recent survey by Ji shows that almost all songs played have beat rates below 2.8Hz. The DLFs for the different activities are presented as follows according to Bachmann. 14 WILFORD, Michael. An Investigation into Crowd-Induced Vertical Dynamic Loads Using Available Measurements. Ove Arup and Partners International Ltd., 2003. 630 Structural Engineering Analysis and Design Second Edition Activity Jumping Dancing Hand clapping with body bouncing while standing Hand clapping Lateral Body Swaying Activity Rate (Hz) Normal 2.0Hz Normal 3.0Hz High 2.0Hz High 3.0Hz 2.0Hz to 3.0Hz 1.6Hz 2.4Hz Normal 1.6Hz Normal 2.4Hz Intensive 2.0Hz Seated 0.6Hz Standing 0.6Hz 1st Harmonic DLF 1.8 1.7 1.9 1.8 0.50 0.17 0.38 0.024 0.047 0.170 DLF½ = 0.4 DLF½ = 0.5 2nd Harmonic DLF 1.3 1.1 1.6 1.3 0.15 0.10 0.12 0.010 0.024 0.047 3rd Harmonic DLF 0.7 0.5 1.1 0.8 0.10 0.04 0.02 0.009 0.015 0.037 First Harmonic 0.50 (1.5 – 3Hz) 0.40 (1.5 – 3Hz) 1.50 (1 – 2.75 Hz) 0.50 (2 – 3 Hz) 0.37 Second Harmonic 0.050 (3 – 6 Hz) 0.150 (3 – 6Hz) 0.600 (2 – 5.5 Hz) 0.150 (4 – 6 Hz) 0.120 Third Harmonic -------0.10 (3 – 8.25 Hz) 0.10 (6 – 9 Hz) 0.04 0.05 (1 –1.5 Hz) 0.25 (1 –1.5 Hz) 0.040 (1.5 – 3 Hz) 0.035 (1.5 – 3 Hz) Not critical Not critical Other guides give the following DLF values. Activity NBCC Dancing NBCC Lively concert or sport event NBCC Jumping/Aerobics CEB 209 Dancing CEB 209 Hand Clapping with body bouncing while standing (2.4 Hz) Horizontal: Front to Back Horizontal: Side to Side Willford (2003) proposed the following vertical DLFs (for jumping at pop concerts) and lateral DLFs. Excitation Frequency (Hz) 1.5 to 3.0 3.0 to 6.0 6.0 to 9.0 Excitation Frequency (Hz) 1.0 to 1.5 1.5 to 3.0 3.0 to 4.5 Vertical Dynamic Load Factor (DLF) 1.50 0.60 0.10 Lateral (Front to Back) Dynamic Load Factor (DLF) 0.05 0.04 Not critical Coefficient of Variation 0.15 0.60 1.00 Lateral (Side to Side) Dynamic Load Factor (DLF) 0.250 0.035 Not critical A forced frequency response analysis SOL 108 or SOL 111 should be carried out in MSC.NASTRAN with all nodes representing the excitations of individual people be incorporated simultaneously within one analysis. Each person induces an excitation in phase with each other, as the most critical case. Hence only one RLOAD entry is required whilst the DAREA card points to all the nodes where a single person may be jumping. This hence models the crowd induced loading and includes exactly the phase difference between the natural modes. This can be used to evaluate exactly the steady-state acceleration response, steady-state displacement response and the steady-state stress and force quantities for structural integrity. 631 Structural Engineering Analysis and Design Second Edition As hand verification, a single modal response analysis may be performed. The modal frequency and modal mass can be obtained from a real modal analysis whilst the damping can be ascertained from a complex modal analysis or from measured data. Then, the modal force can be ascertained from ∫ φ (Ω){P(Ω, t)}dΩ Modal Force = i Ω Amplitude of mod al force, p 0i = ∫ φ (Ω) x DLF x Static Load dΩ Ω i The steady-state (i.e. peak) single mode acceleration response can then be estimated in physical coordinates as a peak = φ response ω2 p0 ωni M i 2 (1 − ω 1 2 / ωni ) 2 2 + (2ζ i ω / ωni ) 2 The following vibration acceptance criteria are proposed for severe dynamic loading cases. These are based on vertical limits proposed by Kasperski (1996) and on the relative sensitivity of humans to lateral and vertical vibration from ISO 2631. Vertical modes: peak acceleration to be less than 18% to 35%g maximum vertical deflection amplitude 10mm. peak acceleration to be less than 6% to 12%g Horizontal modes: The lower numbers are reasonable design targets. Exceedance of the higher values (35%g vertically and 12%g horizontally) could lead to panic. It may also be prudent to evaluate the steady-state single mode displacement response and hence the steadystate single mode stress or force response within the structure to determine the structural integrity of the structure. Note that the dynamic response must be supplemented by the mean of the dynamic excitations, i.e. the static weight of the people, and also the static response due to the static loads on the structure. u peak = φ response p0 ω ni M i 2 (1 − ω 1 2 / ω ni ) 2 2 + (2ζ i ω / ω ni )2 632 Structural Engineering Analysis and Design Second Edition 5.2.6 Crowd Induced (Synchronous) Lateral Vibrations 15 Adequate dynamic performance of a bridge requires that I. the lowest lateral natural frequency should be above about 1.5Hz, or II. there must be sufficient damping present such that synchronous lateral excitation does not occur for the crowd densities expected on the bridge. Damping ratio for stability must be The most famous instance of synchronous lateral excitation occurred on the London Millennium Bridge. The bridge structural diagram is that of a shallow suspension bridge, where the cables are as much as possible below the level of the bridge deck to free the views from the deck. Two groups of four 120mm diameter locked coil cables span from bank to bank over two river piers. The lengths of the three spans are 81m for the north span,144m for the main span between the piers and 108m for the south span. The sag of the cable profile is 2.3m in the main span, around six times shallower than a more conventional suspension bridge structure. The tension in the cable is 22.5MN from the dead load. It is estimated that between 80 000 and 100 000 people crossed the bridge during the first day. Analysis of video footage showed a maximum of 2000 people on the deck at any one time, resulting in a maximum density of between 1.3 and 1.5 people per square meter. Unexpected excessive lateral vibrations of the bridge occurred. The movements took place mainly on the south span, at a frequency of around 0.8Hz (the first south lateral mode), and on the central span, at frequencies of just under 0.5Hz and 1.0Hz (the first and second lateral modes respectively). More rarely, movement occurred on the north span at a frequency of just over 1.0Hz (the first north lateral mode). Excessive vibration did not occur continuously, but built up when a large number of pedestrians were on the affected spans of the bridge and died down if the number of people on the bridge reduced, or if the people stopped walking. From visual estimation of the amplitude of the movements on the south and central span, the maximum lateral acceleration experienced on the bridge was between 200 and 250 milli-g .At this level of acceleration a significant number of pedestrians began to have difficulty in walking and held onto the balustrades for support. No excessive vertical vibration was observed. The tests on the Millennium Bridge showed that the lateral force generated by pedestrians is approximately proportional to the response of the bridge. The correlated force per person can be related to the local velocity Vlocal using a lateral walking force coefficient k as kVlocal. The tests indicated the value of k to be approximately 300Ns/m over the frequency range 0.5 to 1.0 Hz. The ith person’s contribution to the modal force is φi kVlocal. Now the local velocity is related to the modal (response) velocity by Vlocal = φi V. Hence the ith person’s contribution to the modal force is φi k φi V = φi2 kV. Hence the modal excitation force generated by N people on the span is Since the lateral excitation force is proportional of the bridge response, there is a damping requirement for stability. The damping force must exceed the excitation force. The modal damping force is 2ωcMV. Thus if the modal damping force is to exceed the modal excitation force 15 DALLARD, FITZPATRICK, FLINT, LE BOURVA, LOW, RIDSDILL SMITH, WILLFORD. The London Millennium Footbridge. The Structural Engineer Journal Volume 79 / No. 22, Institution of Structural Engineers, London, November 2001. 633 Structural Engineering Analysis and Design Second Edition Rearranging and converting to frequency in Hz, the required damping for stability is This can be evaluated if the mode shape and the distribution of pedestrians is known. Assuming the people are uniformly distributed over the whole span, the number of people in the length dL is The summation can be approximated by the continuous integral Assuming the mode shape is sinusoidal and normalized to unity Hence the damping ratio required for stability c here is the damping ratio, ζ not the damping constant Conversely, for a specified amount of damping, the limited number of people to avoid instability is This formula has been derived assuming the pedestrians are uniformly distributed over the whole span and the mode shape is sinusoidal and has been normalized to unity. To estimate the response, the amplitude related correlated excitation can be made equivalent to a negative damping. Damping is proportional to velocity, hence since the excitation is also proportional to the response velocity, it can be equated to a negative damping having a damping ratio The negative damping varies linearly with N. At NL the negative damping equals the actual damping, making the effective damping zero. The effective damping is Finally, the steady-state displacement amplitude of response at resonance is approximately 1/2ceff. 634 Structural Engineering Analysis and Design Second Edition Knowing the density of people expected on the bridge, the number of people N can be calculated by multiplying the density with the area of the deck. The Millennium Bridge was modified to ensure stability for a crowd density of 2.0 people / m2. Although tests indicate that normal walking becomes difficult at densities above about 1.7 people / m2. Designing for this extreme density means the bridge should always have significant positive damping, such that the response will remain comfortable. The pedestrian test results support this approach. Although lateral vibrations occurred from the onset, increasing with pedestrian numbers, the acceleration amplitudes remained acceptably small provided the number of pedestrians was less than NL by a suitable margin. Unless the usage of the bridge was to be greatly restricted, only two generic options to improve its performance were considered feasible. The first was to increase the stiffness of the bridge to move all its lateral natural frequencies out of the range that could be excited by the lateral footfall forces (it is believed to be possible for any frequency below about 1.3Hz, hence a minimum target of 1.5Hz seems reasonable), and the second was to increase the damping of the bridge to reduce the resonant response. On the Millennium Bridge a total of 37 viscous dampers of viscous rate 250000 Ns/m and 4 pairs of tuned mass dampers weighing 2.5 tonnes each were installed for lateral damping. Damping of the first central lateral mode of 0.49 Hz was 20% of critical damping. Another 26 pairs of vertical tuned mass dampers weighing 1 to 3 tonnes were installed for some additional vertical damping. 635 Structural Engineering Analysis and Design Second Edition 5.3 GL, ML Dynamic Influence Line Analysis for Train Excitations on Bridges A single point excitation does not have a spatial variation to it. Resonant response of different modes is likely depending on the location of the point load with respect to the modal eigenvectors and the frequency of excitation with respect to the natural modal frequency. p p ξ i ( t ) = D i ( t ) 0i = D i ( t ) 2 0i Ki ω ni M i {u i ( t )} = {φ i }ξ i ( t ) Lower modes are not necessarily more significant because the modal response depends on the modal force, modal mass and the dynamic amplification. But a lower mode does however have a lower frequency making the modal stiffness smaller, all else being equal, hence making the modal response larger. But even then, of course, the physical response effects can be more critical from less significant modes (i.e. with lower modal responses) due to the inherent shape of the eigenvector even if the scaling factor (i.e. the modal response) is smaller. Now, earthquake excitations are special in the sense that the loading is distributed as it is a function of the excitation acceleration and the mass of the structure. The loading has a fixed spatial location as the mass of the structure of course does not move to another node. The excitation at different nodes on the structure is also in phase with each other as there is only one source of excitation, namely the base acceleration. In this case, due to the nature of the loading being distributed and spatially in phase, the modal participation factor (and hence also the effective mass) is a good measure of the prominence of the natural mode to the base shear. Lower modes will be more significant than higher modes for the base shear because the modal force of higher modes is small (as there is cancellation of the modal force terms as there are positive and negative components of the eigenvector whilst there being excitation in only one direction). But higher modes may well be significant for the local effects, the physical response effects can be more critical from less significant modes (i.e. with lower modal responses) due to the inherent shape of the eigenvector even if the scaling factor (i.e. the modal response) is smaller. Train excitations are special in the sense that although the load is distributed, there is a spatial variation to the excitation as the train travels over the bridge. This is equivalent to saying that there is a phase difference for the excitation at different parts of the structure. If there were not to be a phase difference in the excitation between different points, the train would have to be jumping vertically at the same spatial location. Consider two random points of a bridge. The wheels of the train will in general travel over these two points at different instances even if we consider the distance between the wheels to be constant (although in reality it is not), unless in the special case the distance between the wheels is equal to the distance of the two nodes we are considering. Because of this phase difference in excitation, it is impossible to excite any modes of the bridge resonantly from a passing train. The solution is best performed in the time domain to include both the transient and steady state response due to a train passing. Time history curves for every node within the path of the train will have to be defined according to the speed of the train and the distance between the wheels. The loading of the passing train on a particular node can be represented by a time history with spikes each time a wheel passes over it. A perfect model will include the equivalent nodal loading whilst a wheel is between two adjacent nodes, hence making the loading time history on the nodes less spiky and more realistic. But if these equivalent nodal loading is not to be considered, then an estimate of the frequency of the impulse must be made. The time lapse between the peaks on the time history at a particular node is of course dependent upon the speed of the train and the distance between the wheels. In this problem, static loads refer to the static weight under gravity of the bridge, and dynamic loads refer to the forces exerted by the wheels of the train onto the bridge. The loading of the passing train on a particular node can be represented by a time history with spikes each time a wheel passes over it. The amplitude of these spikes are the static weight of the train over the particular wheel. Considerations of equivalent nodal loading would result in a time varying load history that rises and falls about a mean load. This mean load is automatically taken into account in time domain analyses, but has to be applied separately if the analysis were to be performed in the frequency domain. 636 Structural Engineering Analysis and Design Second Edition In this LINEAR TIME DOMAIN solution, the static response must be added to the dynamic response if the dynamic analysis is performed about the initial undeflected (by the static loads) state with only the dynamic loads applied, hence causing the dynamic response to be measured relative to the static equilibrium position. Hence, the total response = the dynamic response + the static response to static loads. Alternatively, in this LINEAR TIME DOMAIN solution, if the dynamic analysis is performed with the deflected static shape as initial input and the static loads maintained throughout the dynamic excitations, the total or absolute response (static and dynamic) is obtained straight away from the dynamic analysis. Hence total response = dynamic response (which already includes the static response to static loads). A frequency domain solution may be used, but it may be argued that the starting transient is more significant than the steady-state response, or at least significant. The excitation frequency and excitation phase difference would have to be defined for every node within the path of the train according to the speed of the train, the distance between the wheels and the location of the nodes with respect to each other. Of course, the frequency domain solution will be much faster, but does not include the starting transient and the effects at a particular time i.e. time dependent response cannot be determined (for instance the deflections, slope or cant of the track at a particular time) cannot be established. In this LINEAR FREQUENCY DOMAIN solution, not only that the static response has to be added separately, but also the mean of the dynamic excitation has also got to be added separately as a static response. This is because the mean of the dynamically applied force is not included in the dynamic excitations. Hence the total response in this frequency domain dynamic analysis = static response to mean of dynamic excitation + dynamic response + static response to static loads. As for the speed of the train, it is impossible to generalize the most critical speed. One would think that in order to excite a particular mode critically (chosen such that it has a significant vertical component), one would run the train over the bridge at a speed such that speed of train = distance between wheels / period of mode. But since the excitation is not in phase with each other at different spatial locations along the path, this may not be the critical case. Of course it is prudent to run the train amongst others at the maximum possible speed and such that speed of train = distance between wheels / period of mode. A complication that arises in both the time and frequency domain is that in reality the spacing between the wheels of the train is not constant, hence requiring a more complicated loading definition. The model of the rail could include some smeared mass from the train, as that will contribute to the local frequencies and the dynamic response. Apart from that, it is mandatory that not only translational stiffnesses are used for the rail pads, but also rotational stiffnesses (except in the plane of shells) to connect the rails into the shells representing the deck. This is to fully couple the beams representing the rails to the deck. If this was not done, then the accuracy of the response on the rail beams will be severely compromised. Typical parameters are presented. Property Rail Pads On Solid Concrete Ground Rail Pads On Ballast Vanguard Pads Booted Sleeper Stiffness (N/m) Z – 90.0E6 X and Y – 10.0E6 Z – 70.0E6 X and Y – 10.0E6 Z – 12.5E6 Y – 20.0E6 X – 3.1E6 Z – 42.0E6 X and Y – 10.0E6 637 Structural Damping (Loss Factor) 0.40 0.40 0.40 0.40 Structural Engineering Analysis and Design Second Edition Typical train loadings are presented. This translates to the following load excitation at a particular node representing the force on one wheel end, hence, half the above magnitudes since they represent the weight of the entire wheel axle. The vertical acceleration response criteria at the train deck for passenger comfort set out by the by the UK CTRL is 0.5ms-2. 638 Structural Engineering Analysis and Design Second Edition 5.4 GL, ML Fluid (Wind & Water) - Structure Interaction (Aeroelastic Response Analysis) Flow induced vibrations include: (I) Static Aeroelastic Response (i) Along-Flow Drag (ii) Across-Flow Lift (iii) Torsional Divergence (II) Dynamic Aeroelastic Response (i) Along- and Across-Flow Unsteady Inertial Force Response (ii) Along-Flow Gust Response (iii) Along-Flow Buffeting Response (iv) Across-Flow Von Karman Vortex Shedding Induced Response (III) Dynamic Aeroelastic Stability (i) Across-Flow Galloping (ii) Across-Flow Classical Flutter Apart from these, bodies within fluid are also subject to (I) Upward buoyancy forces (II) All direction atmospheric pressure 10kPa (III) All direction hydrostatic forces ρ.g.(depth in fluid) (IV) Downward gravitational forces 639 Structural Engineering Analysis and Design Second Edition 5.4.1 5.4.1.1 Elementary Hydraulics Pipeline Design (Application of the Steady and Unsteady Bernoulli’s Equation) 640 Structural Engineering Analysis and Design Second Edition 641 Structural Engineering Analysis and Design Second Edition 642 Structural Engineering Analysis and Design Second Edition 643 Structural Engineering Analysis and Design Second Edition 644 Structural Engineering Analysis and Design Second Edition 645 Structural Engineering Analysis and Design Second Edition 646 Structural Engineering Analysis and Design Second Edition 647 Structural Engineering Analysis and Design Second Edition 648 Structural Engineering Analysis and Design Second Edition 649 Structural Engineering Analysis and Design Second Edition 650 Structural Engineering Analysis and Design Second Edition 651 Structural Engineering Analysis and Design Second Edition 652 Structural Engineering Analysis and Design Second Edition 653 Structural Engineering Analysis and Design Second Edition 654 Structural Engineering Analysis and Design Second Edition 655 Structural Engineering Analysis and Design Second Edition 656 Structural Engineering Analysis and Design Second Edition 657 Structural Engineering Analysis and Design Second Edition 658 Structural Engineering Analysis and Design Second Edition 659 Structural Engineering Analysis and Design Second Edition 660 Structural Engineering Analysis and Design Second Edition 661 Structural Engineering Analysis and Design Second Edition 662 Structural Engineering Analysis and Design Second Edition 663 Structural Engineering Analysis and Design Second Edition 664 Structural Engineering Analysis and Design Second Edition 665 Structural Engineering Analysis and Design Second Edition 666 Structural Engineering Analysis and Design Second Edition 667 Structural Engineering Analysis and Design Second Edition 668 Structural Engineering Analysis and Design Second Edition 669 Structural Engineering Analysis and Design Second Edition 670 Structural Engineering Analysis and Design Second Edition 671 Structural Engineering Analysis and Design Second Edition 672 Structural Engineering Analysis and Design Second Edition 673 Structural Engineering Analysis and Design Second Edition 674 Structural Engineering Analysis and Design Second Edition 675 Structural Engineering Analysis and Design Second Edition 676 Structural Engineering Analysis and Design Second Edition 677 Structural Engineering Analysis and Design Second Edition 678 Structural Engineering Analysis and Design Second Edition 679 Structural Engineering Analysis and Design Second Edition 680 Structural Engineering Analysis and Design Second Edition 681 Structural Engineering Analysis and Design Second Edition 682 Structural Engineering Analysis and Design Second Edition 683 Structural Engineering Analysis and Design Second Edition 684 Structural Engineering Analysis and Design Second Edition 685 Structural Engineering Analysis and Design Second Edition 686 Structural Engineering Analysis and Design Second Edition 687 Structural Engineering Analysis and Design Second Edition 688 Structural Engineering Analysis and Design Second Edition 689 Structural Engineering Analysis and Design Second Edition 690 Structural Engineering Analysis and Design Second Edition 691 Structural Engineering Analysis and Design Second Edition 692 Structural Engineering Analysis and Design Second Edition 693 Structural Engineering Analysis and Design Second Edition 694 Structural Engineering Analysis and Design Second Edition 695 Structural Engineering Analysis and Design Second Edition 696 Structural Engineering Analysis and Design Second Edition 697 Structural Engineering Analysis and Design Second Edition 698 Structural Engineering Analysis and Design Second Edition 699 Structural Engineering Analysis and Design Second Edition 700 Structural Engineering Analysis and Design Second Edition 701 Structural Engineering Analysis and Design Second Edition 702 Structural Engineering Analysis and Design Second Edition 703 Structural Engineering Analysis and Design Second Edition 704 Structural Engineering Analysis and Design Second Edition 705 Structural Engineering Analysis and Design Second Edition 706 Structural Engineering Analysis and Design Second Edition 707 Structural Engineering Analysis and Design Second Edition 708 Structural Engineering Analysis and Design Second Edition 709 Structural Engineering Analysis and Design Second Edition 710 Structural Engineering Analysis and Design Second Edition 711 Structural Engineering Analysis and Design Second Edition 712 Structural Engineering Analysis and Design Second Edition 713 Structural Engineering Analysis and Design Second Edition 714 Structural Engineering Analysis and Design Second Edition 715 Structural Engineering Analysis and Design Second Edition 716 Structural Engineering Analysis and Design Second Edition 717 Structural Engineering Analysis and Design Second Edition 718 Structural Engineering Analysis and Design Second Edition 719 Structural Engineering Analysis and Design Second Edition 720 Structural Engineering Analysis and Design Second Edition 721 Structural Engineering Analysis and Design Second Edition 722 Structural Engineering Analysis and Design Second Edition 723 Structural Engineering Analysis and Design Second Edition 724 Structural Engineering Analysis and Design Second Edition 5.4.1.2 5.4.1.2.1 Elementary Wave Mechanics (Small Amplitude Wave Theory) Introduction Wave number, k = 2π/L or 2π/λ, L or λ is the wave length Wave frequency, σ = 2π/T, T = wave period Wave amplitude, a measured from crest to still water level Water depth, d Water surface, η Wave speed, c = λ/T = σ/k Wave height, h = 2a Small amplitude wave theory assumes mass continuity (incompressible fluid), irrotationality (no friction hence invalid in boundary layer near sea bed), unsteady Bernoulli, motion is periodic in x and t, a << λ and a << d. 725 Structural Engineering Analysis and Design Second Edition 5.4.1.2.2 Basic Formulae 726 Structural Engineering Analysis and Design Second Edition 727 Structural Engineering Analysis and Design Second Edition 5.4.1.2.3 Formulae for Special Cases 728 Structural Engineering Analysis and Design Second Edition 729 Structural Engineering Analysis and Design Second Edition 5.4.1.2.4 Formulae for Analysis 730 Structural Engineering Analysis and Design Second Edition 731 Structural Engineering Analysis and Design Second Edition 5.4.2 Static Aeroelastic Response The structural load distribution on an elastic vehicle in trimmed flight is determined by solving the equations for static equilibrium. The SOL 144 and SOL 200 processes will calculate aerodynamic stability derivatives (e.g., lift and moment curve slopes and lift and moment coefficients due to control surface rotation) and trim variables (e.g., angle of attack and control surface setting) as well as aerodynamic and structural loads, structural deflections, and element stresses. 732 Structural Engineering Analysis and Design Second Edition 5.4.2.1 Along-Flow Direction Drag (Pressure Drag and Skin-Friction Drag) (Limited Amplitude Response) The drag forces objects immersed in fluids, can be thought of as being comprised of two parts: Skin-friction Dτ – the forces applied by shearing as the liquid passes the solid boundaries. Pressure-drag DP – the net forces applied to the body due to differences in the upstream and downstream pressure fields. Broadly speaking, both components of the total drag force increase with fluid velocity V. where n is in the range 1.2→1.8 Dτ ∝ Vn DP ∝ V2 The relative magnitude of these two drag components depends on the geometry of the object in the fluid. For ‘stream-lined’ bodies e.g. a flat plate parallel to the flow direction, the drag will be almost entirely skin friction while for ‘bluff’ bodies e.g. a flat plate normal to the flow direction, the pressure drag will dominate. For some cross-sections e.g. a cylinder, the ratio of these two drag forces varies considerably depending on the flow regime. But the skin friction drag is usually of a much smaller magnitude even for streamlined bodies. The (pressure and skin friction) drag on a body immersed in a steady fluid flow can be expressed by a dimensionless quantity known as the drag coefficient, CD, such that the total drag force on the body is given by 1 F = ρV 2 .C D .Area 2 The flow regime around a body is governed by a dimensionless quantity known as the Reynold’s Number, Re. This dimensionless quantity is defined as the ratio of inertial to viscous forces in a fluid. The non-dimensional Reynolds Number is defined for the flow around a cylinder as Re = ρVD µ where ρ is the fluid density, V the stream velocity relative to the cylinder, D the diameter of the cylinder and µ the dynamic viscosity of the fluid. 733 Structural Engineering Analysis and Design Second Edition At small Re < 0.5, the inertia effects are negligible and glow pattern very similar to ideal flow, the pressure recovery being nearly complete. Pressure drag negligible and total profile drag is nearly all due to friction drag. Here, CD and Re exhibit a straight line from which we can conclude that drag is directly proportional to the velocity V (Stoke’s Law). At 2 < Re < 30, separation of boundary layers occur. The boundary layer is laminar. Two symmetrical eddies rotating in opposition to each other are formed. They remain fixed in position and the main flow closes behind them. The separation of the boundary layer is reflected in the graph of CD versus Re by the curvature of the line indicating that the drag is now proportional to Vn where n 2. Further increase in Re (90 < Re < 2 x 105) tends to elongate the fixed eddies. At Re of 90 onwards, the eddies break away from the cylinder. The separation point moves to an earlier point. The boundary layer is laminar. The breaking away occurs alternately from one and then the other side of the cylinder, the eddies being washed away by the mainstream. This process is intensified by further increase in Re, whereby the shedding of the eddies from alternate sides of the cylinder is continuous, thus forming in the wake two discreet rows of vortices. This is known as vortex street or von Karmon vortex street. The shedding of these vortices produces circulation and hence gives rise to lateral forces on the cylinder. It is fortunate that at higher Re (Re > 2 x 105) values the vortices disappear because of high rates of shear and are then replaced by a highly turbulent wake. The boundary layer changes to turbulent (instead of laminar) before separation. The effect of this is that the separation point moves later instead of the general trend of moving to an earlier point. Hence a smaller wake results, and thus reduced drag. Regular vortex shedding occurs, not alternating anymore. Roughness becomes important at high Re in determining CD. At Re > 107, the value of CD appears to be independent of Re, but there is insufficient data at this end of the range. An explanation of the boundary layer formation and its separation is warranted. For real fluids, a thin boundary layer grows from the stagnation point at A. The boundary layer is a layer of fluid near the surface of the body which is affect is affected by shear forces, hence friction is prominent and ideal flow theories do not hold. A to B is the region of velocity increasing in x (acceleration), hence the pressure decreases in x i.e. a favourable pressure gradient as the boundary layer tends to reduce in thickness. From B to C, the velocity decreases in x (deceleration), hence the pressure increases in x i.e. an adverse pressure gradient as the boundary layer thickens. This force which opposes the direction of fluid motion coupled with the action of the shear forces in the boundary layer if they act for a sufficient length will bring the fluid in the boundary layer to rest and subsequently the flow separates from the surface of the body. When the fluid near the surface begins to move in the other direction due to the adverse pressure gradient, this implies that the boundary layer (i.e. the point where the fluid is zero velocity) separates from the surface. This flow separation has serious consequences in aerofoil design as once the flow separates away from the surface, all lift is lost. B A x C Flow in the wake is highly turbulent and consists of large scale eddies. High rate energy dissipation occurs with the result of a pressure reduction in the wake. But the stagnation pressure in front is high and thus the resultant force arising from pressure difference is called the drag force. The bigger the wake (i.e. the earlier the boundary layer separation point), the smaller the pressure in the wake and so the greater the pressure drag. 734 Structural Engineering Analysis and Design Second Edition 5.4.2.2 Across-Flow Direction Lift (Pressure Lift and Skin-Friction Lift) (Limited Amplitude Response) The (pressure and skin friction) lift is analogous to the drag and acts in the direction perpendicular to the direction of fluid motion. 1 F = ρV 2 .C L .Area 2 Lift occurs when the faster moving fluid on top of the aerofoil has a lower pressure to the slower moving fluid underneath. If the boundary layer separation occurs at the top of the aerofoil, the suction pressure is lost. This is known as stalling. The plane will then drop from the sky. The only solution is to put the plane in a dive to regain the boundary layer. The two dimensional drag and lift coefficients for structural shapes are presented. Clearly, the lift is zero for a body symmetrical about the direction of flow. 735 Structural Engineering Analysis and Design Second Edition 5.4.2.3 Non-Oscillatory Torsional Divergence (Divergent Amplitude Response) Divergence can occur if the aerodynamic torsional stiffness (i.e. the rate of change of pitching moment with rotation) is negative. At the critical wind speed the negative aerodynamic stiffness becomes numerically equal to the structural torsional stiffness resulting in zero total stiffness. Torsional divergence is an instance of a static response of a structure. Torsional divergence was at first associated with aircraft wings due to their susceptibility to twisting off at excessive air speeds (Simiu and Scanlan, 1986). Liu, 1991, reports that when the wind flow occurs, drag, lift, and moment are produced on the structure. This moment induces a twist on the structure and causes the angle of incidence α to increase. The increase in α results in higher torsional moment as the wind velocity increases. If the structure does not have sufficient torsional stiffness to resist this increasing moment, the structure becomes unstable and will be twisted to failure. Simiu and Scanlan, 1986, report that the phenomenon depends upon structural flexibility and the manner in which the aerodynamic moments develop with twist; it does not depend upon ultimate strength. They say that in most cases the critical divergence velocities are extremely high, well beyond the range of velocities normally considered in design. 736 Structural Engineering Analysis and Design Second Edition BD 49/01 (valid depending on the aerodynamic susceptibility parameter, Pb and satisfying some geometric constraints) the states that a bridge is unsusceptible to non-oscillatory torsional divergence if it is stable against self-induced instability, i.e. galloping (and stall flutter) and classical flutter. 737 Structural Engineering Analysis and Design Second Edition BD 49/01 is valid depending on the value of the aerodynamic susceptibility parameter, Pb where ρ is the density of air, b is the overall width of the bridge deck, m is the mass per unit length of the bridge, Vr is the hourly mean wind speed (for relieving areas), L is the length of the relevant maximum span of the bridge and fB is the natural frequency in bending. Then (a) If Pb < 0.04, bridge is subject to insignificant effects in respect of all forms of aerodynamic excitation. (b) Bridges having 0.04 ≤ Pb ≤ 1.00 shall be considered to be within the scope of the BD 49/01 rules. (c) Bridges with Pb > 1.00 shall be considered to be potentially very susceptible to aerodynamic excitation and are thus beyond the scope of BD 49/01. Further analytical and/or wind tunnel tests must be performed. Normal highway bridges of less than 25m span should generally be found to be category (a). Bridges of spans greater than 250m are likely to be category (c). Covered footbridges, cable supported bridges and other structures where any of the parameters b, L or fB cannot be accurately derived shall be considered as category (c). For the purposes of initial/ preliminary categorisation, the following may be used to given an indicative range for Pb: Vr between 20 and 40 m/s; m/b between 600 and 1200 kg/m2; fB between 50/L0.87 and 100/L0.87, with L in metres.. The geometric constraints for the applicability of BD 49/01 are detailed. (i) Solid edge members, such as fascia beams and solid parapets shall have a total depth less than 0.2d4 unless positioned closer than 0.5d4 from the outer girder when they shall not protrude above the deck by more than 0.2d4 nor below the deck by more than 0.5d4. In defining such edge members, edge stiffening of the slab to a depth of 0.5 times the slab thickness may be ignored. (ii) Other edge members such as parapets, barriers, etc., shall have a height above deck level, h, and a solidity ratio, φ, such that φ is less than 0.5 and the product hφ is less than 0.35d4 for the effective edge member. The value of φ may exceed 0.5 over short lengths of parapet, provided that the total length projected onto the bridge centre-line of both the upwind and downwind portions of parapet whose solidity ratio exceeds 0.5 does not exceed 30% of the bridge span. (iii) Any central median barrier shall have a shadow area in elevation per metre length less than 0.5m2. Kerbs or upstands greater than 100mm deep shall be considered as part of this constraint by treating as a solid bluff depth; where less than 100mm the depth shall be neglected, see figure below. In the above, d4 is the reference depth of the bridge deck. Where the depth is variable over the span, d4 shall be taken as the average value over the middle third of the longest span. 738 Structural Engineering Analysis and Design Second Edition 739 Structural Engineering Analysis and Design Second Edition 5.4.3 Dynamic Aeroelastic Response Aeroelastic analysis concerns the interaction of aerodynamic and structural (inertial, damping and stiffness) forces. It is utilized in the design of airplanes, suspension bridges, missiles, power lines, tall chimneys etc. 5.4.3.1 Along- and Across-Flow Direction Unsteady Inertial Forces on General Submerged Structures Due to Water Waves (Limited Amplitude Response) Based on small amplitude wave mechanics, the unsteady (time varying) pressure distribution under the surface of the fluid on a general submerged structure due to waves is p= ρga cosh k ( y + d ) sin(σt − kx ) cosh kd where ρ = density of fluid a = amplitude of waves k = 2π/L, where L is the wavelength y = height above fluid surface, measure positive upwards d = total depth of fluid σ = 2π/T, where T is the wave period This pressure expression is integrated with respect to y from –d to 0 for the total force. 740 Structural Engineering Analysis and Design Second Edition 5.4.3.2 Along- and Across-Flow Direction Unsteady Inertial Forces on Cylindrical Submerged Structures Due to Water Waves (And Along-Flow Direction Drag Forces Due to Steady Currents) (Limited Amplitude Response) The unsteady inertial force on a cylinder is given by 1 ∂u F = ρπ.d 2 .C M . ( Force per length) 4 ∂t CM is the inertial coefficient which varies depending upon the degree of flow separation and wake formation. Experimental measurements have shown that the amplitude of the fluid motion relative to the diameter of the cylinder has an important effect on the nature of the induced loading. The ratio is defined as the KeuleganCarpenter number. The KC number is really the drag versus inertia ratio. KC = uT/d where u is the velocity amplitude, T the period of oscillatory motion and d the diameter of the cylinder. This characterizes the Morrison’s equation which includes the steady drag force and the unsteady inertial force. F= 1 1 ∂u ρV 2 .C D .d + ρπ.d 2 .C M . 2 4 ∂t (Force per length) Coefficients 2.0 CM 1.0 0.0 CD 10 20 30 40 KC 50 For small KC, the velocity amplitude is small relative to the diameter of the cylinder. Flow does not separate fully and thus in the limiting case where KC is very small the flow becomes potential flow. Hence the drag coefficient reduces to 0.0 and the inertial coefficient becomes 2.0 (idealized case). For large KC, the velocity amplitude is larger than the cylinder diameter. Both inertial and drag forces are important. However since the drag is proportional to V2, this will produce the dominant contribution to Morison’s equation. 741 Structural Engineering Analysis and Design Second Edition 742 Structural Engineering Analysis and Design Second Edition 743 Structural Engineering Analysis and Design Second Edition 5.4.3.3 Along-Flow Direction Gust Response (And Along-Flow Direction Drag Forces Due to Steady Mean Wind) (Limited Amplitude Response) The total wind velocity is Utotal (z, t) = Umean (z) + Ugust (z, t) The mean velocity is defined Umean (z) = U10 . (z / 10)α where U10 is the reference mean wind speed at 10m above ground and α is the roughness coefficient α = 0.16 for open country α = 0.28 for woods, villages and towns α = 0.40 for large city centres Note that U10 usually lies between 24 and 34ms-1. The mean velocity gives rise to the steady drag force. The gust gives rise to the dynamic gust response. The spectral density of the gust is defined as follows. Gust spectral density = Gust spectrum x (Aerodynamic admittance function)2 The gust spectrum is the wind speed spectra at a particular point. The aerodynamic admittance function defines the relationship between the gust frequency and its area of influence. Gusts of higher frequency have a smaller area of influence and vice versa. The gust spectral density function usually exhibit peak frequencies between 0.05 and 0.1Hz. Passive tuned mass dampers offer little to reducing gust response due to the impulsive nature of the excitation. Stiffening the structure is the usual effective approach. For design purposes, as described in codes of practise, the wind force due to both mean speed and gust can be obtained using the equivalent static wind force W = ϕ . cf . q . A where ϕ = gust factor cf = aerodynamic resistance coefficient q = wind drag pressure = ρUmean2/2 A = area loaded The gust factor ϕ considers both the stochastically varying aerodynamic properties of the natural wind and the vibration behaviour of the structure in its fundamental mode as is given by ϕ = 1 + R (B + s.F/Λ)0.5 where R = terrain factor = function (α) B = basic gust factor = function (d, h) d = width of structure h = height of structure s = size factor = function (f.h/Uh,d/h) F = gust energy factor = function (f/Uh) f = structural fundamental frequency in wind direction Uh = mean wind speed at height h Λ = damping (expressed as logarithmic decrement) of the fundamental mode In BS 6399-2, the pressure and skin friction drag is respectively where Cf is the friction drag coefficient, As is the area swept by the wind and Cr is the dynamic augmentation factor 744 Structural Engineering Analysis and Design Second Edition where Sg is the gust factor. The pressure drag force is The (internal and external) pressures, p applied on the structure are calculated from p = q s . Cp . C a where Cp is the (internal or external) pressure coefficient, Ca is the size effect factor and the dynamic wind pressure, qs is qs = 0.613Ve2 where the (structure dependent) effective wind speed, Ve is Ve = Vs . Sb where Sb = the terrain factor Vs = (site dependent) site wind speed = Vb . Sa . Sd . Ss . Sp where Vb = (area dependent) basic hourly mean wind speed at 10m height above sea level Sa = altitude factor Sd = direction factor Ss = seasonal factor Sp = probability factor The skin friction drag is ignored. Only the more significant pressure drag is accounted for. For the site of Metz which is in Department Moselle, i.e. Zone 2, corresponding basic wind speed (reference EC1) is Vb = 26 m/s The site wind speed Vs = Vb . Sa . Sd . Ss . Sp ≈ 26 m/s where the altitude factor, Sa ≈ 1.0 (non significant topographical effects) the direction factor, Sd = 1.0 (wind direction III – 210°) the seasonal factor, Ss = 1.0 (since it is a permanent building and hence exposed for at least 6 months) the probability factor, Sp = 1.0 (for standard 2% probability of exceedance) The structure dependent effective wind speed, Ve is Ve = Vs . Sb = 48 m/s where the terrain and building factor (taking effective height, He = 30m conservatively as the whole height and assuming site in town >100km to closest distance to sea) is Sb = 1.85 745 Structural Engineering Analysis and Design Second Edition The dynamic wind pressure, qs is thus qs = 0.613Ve2 = 1.42 kPa The pressure, p applied on the structure is thus p = q s . Cp . C a = qs.(Cpe-Cpi).Ca = 1.106(Cpe-Cpi) where the size effect factor (taking the loaded area diagonal, a = (902 + 302)0.5 = 95m and assuming site in town >100km to closest distance to sea) is Ca = 0.78 746 Structural Engineering Analysis and Design Second Edition where the external pressure coefficient Cpe for duo-pitch roofs is obtained from as follows 747 Structural Engineering Analysis and Design Second Edition The scaling lengths bL and bW where bL = L or bL = 2H, whichever is the smaller, and bW = W or bW = 2H, whichever is the smaller. External pressure can be negative for low-pitched roofs while it becomes positive for higher pitches. For a +60° roof, on average we have +0.8 on the side facing the wind and –0.65 on the side not facing the wind. The asymmetric load case must be applied. External pressure coefficients for mansard roofs and other multi-pitch roofs should be derived for each plane face by the procedure given for duo-pitch roofs. 748 Structural Engineering Analysis and Design Second Edition The external pressure coefficient Cpe for flat roofs is obtained from 749 Structural Engineering Analysis and Design Second Edition The coefficients for hipped roofs are presented. 750 Structural Engineering Analysis and Design Second Edition 751 Structural Engineering Analysis and Design Second Edition The external pressure coefficient Cpe for building walls is obtained from 752 Structural Engineering Analysis and Design Second Edition The internal pressure coefficient Cpi for roofs and buildings is obtained from the following for buildings with dominant openings The internal pressure coefficients for enclosed buildings is Pressure coefficients are considered positive when pressure is acting on the surface (i.e. normal to the surface) of structure and negative when the pressure is acting away from the surface (still normal to the surface). Hence positive external pressure acts inward on structure and positive internal pressure acts outward on structure, and vice versa. It is important then to apply pressure loads in the local coordinate system of the element in a finite element program and not in the global axes system. Internal pressure occurs due to openings such as windows, doors, vents and cladding. In general if the windward panel has a greater opening than the leeward panel, more wind comes in than out and hence the interior is subject to positive (outward of building) pressure, and vice versa. Note that the net pressure coefficient, Cp for buildings is Note that the net pressure coefficient, Cp on a free−standing signboard is 1.8. Note that the net upward pressure coefficient, Cp on a canopy is 1.8. 753 Structural Engineering Analysis and Design Second Edition 754 Structural Engineering Analysis and Design Second Edition 755 Structural Engineering Analysis and Design Second Edition Note that the net pressure coefficients, Cp on long cylinders and sharp edged elements such as rolled sections, plate girders and boxes are Finally, the design pressure is pdesign = 0.85[1.106(Cpe-Cpi)].(1+Cr) where the dynamic augmentation factor Cr is given by The gust factor is Sg = 1 + gtStTt = 1.52 obtained from 756 Structural Engineering Analysis and Design Second Edition gust peak factor, gt = 2.30 (for He ~ 30m, a ~ 95m) (Table 24) turbulence factor, St = 0.159 (for He ~ 30m, site >100m from sea) (Table 22) turbulence adjustment factor, Tt = 1.43 (for He ~ 30m, upwind distance from edge of town > 30m) (note Tt = 1 for country site) (Table 23) Now, where terrain correction factor, Kt = 0.75 (since town site; 1.33 if sea coast) and the terrain and building factor 757 Structural Engineering Analysis and Design Second Edition SO = ScTc(1+Sh) = 0.996 obtained from the fetch factor, Sc = 1.2 (Table 22) the fetch adjustment factor, Tc = 0.83 (Table 23) topographic increment, Sh = 0 (for flat sites) Hence, Kh x Kb = 0.75 x (20 x 0.996 / (no2 x 95))2/3 x (26/(24ζ)) = 0.287 (1/no2)2/3 (1/ζ) where no is the fundamental natural frequency in Hz and the ζ the viscous damping of critical. Thus the dynamic augmentation factor becomes Cr = 0.567 x [(1+(0.287 (1/no2)2/3 (1/ζ))/60)0.5 − 1] Note that the structure is mildly dynamic for Cr < 0.25, but susceptible to dynamic amplifications in response to the gust if Cr > 0.25 in which case this simplified equivalent static procedure would be less accurate, but generally more conservative. Thus, the design pressure is pdesign = 0.85[1.106(Cpe-Cpi)].(1+Cr) = 0.85[1.106(Cpe-Cpi)].(1+0.567 x [(1+(0.287 (1/no2)2/3 (1/ζ))/60)0.5 − 1]) To ensure that structure not susceptible to dynamic amplifications from gust, need Cr at most 0.25. For assumed damping of critical of ζ = 0.04, thus no must be at least 0.19Hz. At this value of Cr of 0.25, pdesign = 0.85[1.106(Cpe-Cpi)].(1+0.25) = 1.18 (Cpe-Cpi) kPa For comfort criteria, the peak acceleration at the top of a building for resonance in a fundamental bending mode can be estimated from & x&= & x&res (2πn 0 )2 = G res M (2πn 0 )2 M1 where Gres = gust factor for resonant component = g2(σv/V)h(SE/ζ)0.5 M = mean base overturning moment; for a square building, it can be approximated by 0.6 ½ ρVh2bh2 M1 = inertial base bending moment for unit displacement at top of building; for constant density and linear mode shape, = 1/3 ρ bdh2 (2πn0)2 g = peak factor n0 = first bending mode natural frequency; can be approximated by 46/h where h is height in metres (σv/V)h = longitudinal turbulence intensity at height h T = period under consideration, sec; usually 600 sec for acceleration criteria h = height of building b = width of building d = depth of building Vh = hourly mean wind speed at height h S = size factor = 1/[(1+3.5n0h/Vh)(1+4n0b/Vh)] E = longitudinal turbulence spectrum = 0.47N/(2+N2)5/6 N = reduced frequency = nLh/Vh Lh = measure of turbulence length scale = 1000 (h/10)0.25 ρ = air density ρS = building density ζ = critical damping ratio Note that tall buildings have generally SLS and ULS values of reduced velocity (Vh/(n0b)) within the range 2 to 10. Bachmann gives acceleration limits for buildings as follows. 758 Structural Engineering Analysis and Design Second Edition Perception Imperceptible Perceptible Annoying Very Annoying Intolerable Acceleration Limits a < 0.005g 0.005g < a < 0.015g 0.015g < a < 0.05g 0.05g < a < 0.15g a > 0.15g BD 49/01 (valid depending on the aerodynamic susceptibility parameter, Pb and satisfying some geometric constraints) states that provided the fundamental frequencies in both bending and torsion calculated are greater than 1Hz, the dynamic magnification effects of turbulence may be ignored. The dynamic magnification effects of turbulence may also be neglected if PT < 1.0 where (using consistent set of units) and ρ is the density of air, b is the overall width of the bridge deck, m is the mass per unit length of the bridge and fB the natural frequency of bridge in bending. Vs is the site hourly mean wind speed (10m above ground level). σflm is the peak stress in the structure per unit deflection in the first mode of vibration, derived for the most highly stressed location in the relevant element (Units in N/mm²/Unit deflection). σc is a reference stress as follows for steel beam elements, σc = 600 N/mm2 for the longitudinal flange bending stress; for truss bridges, σc = 750 N/mm2 for the chord axial stress; for concrete elements (composite or concrete bridges), σc = 80 N/mm2 for primary bending concrete stress for cable-stayed bridges the peak stay axial stress should additionally be examined, with σc = 1200 N/mm2. The MSC.NASTRAN aeroelastic dynamic response problem determines the response of the aircraft to time or frequency-varying excitations. Atmospheric turbulence is the primary example of this type of excitation, but wind shear and control surface motion can also have an aeroelastic component. Methods of generalized harmonic (Fourier) analysis are applied to the linear system to obtain the response to the excitation in the time domain. The gust response analysis may be regarded either as a stationary random loading or as a discrete gust. The gust analysis capability computes the response to random atmospheric turbulence, discrete one-dimensional gust fields, and control surface motion and other dynamic loading. The random response parameters calculated are the power spectral density, root mean square response, and mean frequency of zero-crossings. The response to the discrete gust and control surface motion is calculated by direct and inverse Fourier transform methods since the oscillatory aerodynamics are known only in the frequency domain. The time histories of response quantities are the output in the discrete case. One subsonic and three supersonic lifting surface aerodynamic theories are available in MSC.Nastran, as well as Strip Theory. The subsonic theory is the Doublet-Lattice method, which can account for interference among multiple lifting surfaces and bodies. The supersonic theories are the Mach Box method, Piston Theory, and the ZONA51 method for multiple interfering lifting surfaces. MSC.Nastran has implemented six aerodynamic theories: 1. Doublet-Lattice subsonic lifting surface theory (DLM) 2. ZONA51 supersonic lifting surface theory 3. Subsonic wing-body interference theory (DLM with slender bodies) 4. Mach Box method 5. Strip Theory 6. Piston Theory The coupling with aerodynamic loads has also been added to the existing MSC.Nastran structural modal frequency response capability, SOL 146. Analyses of frequency response to arbitrarily specified forcing functions can be carried out using the oscillatory aerodynamic loads from many of the available aerodynamic theories. Frequency 759 Structural Engineering Analysis and Design Second Edition response to a harmonic gust field can be calculated at subsonic speeds using the Doublet-Lattice method for wing/body interference, and by the ZONA51 method for interfering lifting surfaces at supersonic speeds. Because unsteady aerodynamic loads are obtained only for steady-state harmonic motion, they are known only in the frequency- and not the time-domain. In SOL 146, Inverse Fourier Transform techniques provide the appropriate methods by which transient response is obtained from the frequency response. Both forward and inverse Fourier transforms are provided so that the time-varying forcing function or the gust profile can be transformed into the frequency domain. Then, after convolution with the system frequency response, the inverse transform leads to the transient response of the system to the specified forcing function or gust profile. Stationary random response of the system, is available in SOL 146 from specified loadings and the power spectral densities of loads. Loads may be either specified force distributions or harmonic gust fields. The statistical quantities of interest in the response are A, the ratio of standard deviations (rms values) of the response to that of the input loading, and N0, the mean frequency of zero crossings (with a positive slope) of the response. The capability to compute these quantities was added to MSC.Nastran by modifying the existing random response module to include options to generate various atmospheric turbulence power spectra and to perform the calculation of N0. Dynamic aeroelasticity differs from the flutter analysis in that the right-hand side of the equation is no longer zero. Instead, loading, which can be in either the frequency or the time domain, is applied. For both types of loading, MSC.Nastran performs the primary analyses in the frequency domain. If the user has supplied loadings in the time domain, Fourier Transform techniques are used to convert the loadings into the frequency domain, a frequency response analysis is performed, and the computed quantities are transformed back to the time domain using Inverse Fourier Transform techniques. Aeroelastic frequency response analysis in MSC.Nastran is performed in modal coordinates and has a basic equation of the form The right-hand side provides the loading in modal coordinates, which can be aerodynamic or nonaerodynamic in nature and is a function of the analysis frequency. Nonaerodynamic generalized loads, designated PHF(w), are obtained in the standard fashion from the loadings applied to physical coordinates. The solution of the equation entails solving for the generalized displacements by decomposition/forward-backward substitution techniques applied to the coupled set of complex equations. Because modal reduction techniques have been applied, the solution costs are typically modest. Once the generalized displacements have been computed, standard data recovery techniques can be used to determine physical displacements, velocities, stress, etc. 760 Structural Engineering Analysis and Design Second Edition 5.4.3.4 Along-Flow Direction Buffeting Response (Limited Amplitude Response) The airflow behind obstacles exhibit increased turbulence which can be of a stochastic nature or a period regular shedding of (von Karman) vortices (defined by the Strouhal number). These vortices give rise to periodic dynamic forces acting on structures that lie within such an air flow. This phenomenon is called buffeting. Note that we are not talking about the response on the obstacle (which may suffer from vortex shedding excitations) but instead on the structures behind, i.e. within the turbulent wake. The ratio of the distance a between the obstacle and the structure and the width d of the obstacle is important. Considerable dynamic effects are obtained from a/d 2 to 16, peaking at about 8. Buffeting can be avoided by stiffening the downwind structure in the air flow. Alternatively, since the wind effect is periodic, its influence can be reduced by increasing damping or using tuned mass dampers, or as with vortex shedding control, Scruton helical stabilizing devices can be used. 761 Structural Engineering Analysis and Design Second Edition 5.4.3.5 Across-Flow Direction Von Karman Vortex Shedding Induced Response (Limited Amplitude Response) Vortex Shedding Frequency When a body is subjected to wind flow, the separation of flow around the body produces forces on the body, a pressure force on the windward side and a suction force on the leeward side. The pressure and suction forces result in the formation of vortices in the wake region. These vortices tend to be shed from alternate sides of the body at Reynold’s number of around 90 to 2 x 105. The large radius (small curvature) vortices produce higher pressures whilst the small radius (large curvature) vortices produce lower pressures, giving rise to alternating lateral forces. Vortex shedding is responsible for the whistling of hanging telephone or power cables. When the frequency of the vortex shedding (aka wake frequency) is close to a prominent natural frequency of the structure, the resulting condition is called lock-in, so-called because the wake frequency remains locked to the natural frequency for a range of wind speeds. During lock-in, the structural member oscillates with increased amplitude but rarely exceeds half the across wind dimension of the body. As the velocity further increases, the wake frequency will again break away from the natural frequency. Lock-in region around natural frequency of structure Wind velocity The vortex shedding phenomena is describable in terms of a non-dimensional Strouhal Number defined as NSD = function of geometry and Reynold' s Number V where NS is the frequency of the vortex shedding, D is the characteristic dimension of the body projected on a plane normal to the mean flow velocity and V the stream velocity. If the shedding frequency is approximately proportional to V, then S is constant. S= The Strouhal number for a cylinder is approximately 0.2 but more accurately  19.7  0.1981   Re  The Strouhal number for other noncircular shapes are presented. 762 Structural Engineering Analysis and Design Second Edition The dynamic response at resonance of a natural structural frequency (with the vortex shedding frequency) can be obtained by multiplying the static response to the lift force 1 F = ρV 2 .C L .Area 2 by the dynamic amplification 1/(2ζ). In other words the dynamic equilibrium equation is 1 m& u&+ cu&+ ku = ρV 2 .C L .Area. sin (2πN s t ) 2 Unfortunately, CL is not constant instead varying with amplitude. Alternatively, the following equation may be used y0/d = 0.123.CL.(1/S2).(1/Sc) where y0 is the displacement amplitude, S the Strouhal number and Sc the Scruton number given by Sc = 2.m.(2πζ)/(ρ.D2) where ζ is the (of critical) damping, m the mass per unit length and D the across flow dimension. Other expressions are presented, here δr is another notation for the Scruton number Sc. Graphs showing estimates of displacement are presented. 763 Structural Engineering Analysis and Design Second Edition As an example, consider a steel circular pile driven vertically into the bed of a river of depth 20m and stream velocity V. The pile dimensions are Outer diameter, D = 0.7m Wall thickness, t = 0.01m Mass of pile in air, mp = 169kg/m I = 1.29E-3 m4 E = 200E9 N/m2 Density of water, ρ = 1020 kg/m3 Added mass of water per unit length = ¼ ρπD2 Damping ratio, ζ = 0.015 Firstly, the critical stream velocities, V at which vortex shedding locks-in to the first two fundamental frequencies are required. Total pile mass per unit length = mass in air + water in hollow pile + added mass of water = 169 + 1020 x ¼ π(0.7-0.02)2 + 1020 x ¼ π(0.7)2 = 931.9 kg/m Effective length of pile adding a fixing length of 6D say = 20 + 6 x 0.7 = 24.2m 3.52 EI 1st natural bending frequency = ≈ 0.50Hz 2π mL4 22 EI 2nd natural bending frequency = ≈ 3.15Hz 2π mL4 Lock in for the 1st mode occurs at V = ND/S = 0.50 x 0.7 / 0.2 = 1.75m/s Lock in for the 2nd mode occurs at V = ND/S = 3.15 x 0.7 / 0.2 = 11.03m/s Secondly, the amplitude of the cross-flow vibrations need to be estimated. This can be performed using the graph presented above. Scruton number, Sc or δr = 2.m.(2πζ)/(ρ.D2) = 2 x 931.9 x (2 x π x 0.015) / (1020 x 0.72) = 0.35 764 Structural Engineering Analysis and Design Second Edition From graph, (A/D)/γ = 1.1 Hence, A1 = 1.1 x 0.7 x 1.305 = 1.0m Hence, A2 = 1.1 x 0.7 x 1.499 = 1.2m The pile is clearly unacceptable due to its susceptibility to vortex shedding for low velocities and due to the large amplitude vortex induced motion. The above proceedings can be most readily applied to a steel chimney stack in a steady wind stream. To avoid vortex shedding, increase structural frequency to avoid resonance, increase structural damping inherent or by using tuned mass dampers or add a vortex suppression device such as a Scruton helical device to ensure vortex shedding lines are no longer vertical lines but spirals and hence reducing the dynamic effect. BD 49/01 (valid depending on the aerodynamic susceptibility parameter, Pb) states that any bridge with fundamental vertical bending or torsional frequency greater than 5Hz shall be stable with respect to vortex shedding. Truss bridges with solidity ratio, φ < 0.5 are also stable against vortex shedding excitations. The solidity ratio is defined as the ratio of the net total projected area of the truss components to the front face of the windward truss over the projected area of encompassed by the outer boundaries of the truss, excluding depth of the deck. Plate girder bridges shall be considered unsusceptible to excitation of the vertical bending or torsional modes if the critical wind speed, Vcr is greater than the reference wind speed, Vvs = 1.25Vr where Vr is the hourly mean wind speed. Otherwise susceptible. The critical wind speed is obtained from below. Note that d4 is the depth of the bridge and b* the effective width. Where the depth is variable over the span, d4 shall be taken as the average value over the middle third of the longest span; is either fB or fT as appropriate, i.e. the natural frequencies in bending and torsion respectively (Hz) calculated under dead and superimposed dead load. 765 Structural Engineering Analysis and Design Second Edition Truss bridges with φ > 0.5 can be evaluated using the plate girder bridge equation by taking d4 as φd4. Eurocode 1-2.4:1995 presents rules for vortex shedding as follows. 766 Structural Engineering Analysis and Design Second Edition 767 Structural Engineering Analysis and Design Second Edition 768 Structural Engineering Analysis and Design Second Edition 769 Structural Engineering Analysis and Design Second Edition 770 Structural Engineering Analysis and Design Second Edition 771 Structural Engineering Analysis and Design Second Edition 772 Structural Engineering Analysis and Design Second Edition 773 Structural Engineering Analysis and Design Second Edition 774 Structural Engineering Analysis and Design Second Edition 775 Structural Engineering Analysis and Design Second Edition 776 Structural Engineering Analysis and Design Second Edition 5.4.4 Dynamic Aeroelastic Stability In this self-induced vibration, the aerodynamic excitation forces depend on the motion of the structure itself. Circular cylinders are not affected by this kind of vibration, but all other sectional shapes are. 5.4.4.1 Across-Flow Direction Galloping and Stall Flutter (Divergent Amplitude Response) Across-wind galloping causes a crosswise vibration in the bridge deck. As the section vibrates crosswise in a steady wind velocity U, the relative velocity changes, thereby changing the angle of attack (α). Due to the change in α, an increase or decrease on the lift force of the cylinder occurs. If an increase of α causes an increase in the lift force in the opposite direction of motion, the situation is stable. But on the other hand if the vice versa occurs, i. e., an increase of α causes a decrease in lift force, then the situation is unstable and galloping occurs. A classical example of this phenomenon is observed in ice covered power transmission lines. Galloping is reduced in these lines by decreasing the distance between spacing of the supports and increasing the tension of the lines. Under certain conditions of profile shape and incidence angle, the so-called aerodynamic damping can be negative and where structural damping is small, galloping instability occurs. It depends on the characteristics of the variation of drag, lift and pitching moment with the angle of incidence. The Glauert-den Hartog instability criterion for galloping is dCL/dα + CD < 0 or since dCy/dα = −[dCL/dα + CD] thus dCy/dα > 0 where CL is the lift coefficient, α is the angle of incidence of the airflow and Cy the force coefficient. This is proven from the mathematics as presented below. From the mathematics, the critical wind speed is given by Ugallop/nD = 2.Sc/(dCy/dα)α=0 777 Structural Engineering Analysis and Design Second Edition where n is the natural structural frequency and the Scruton number (or so-called reduced damping) Sc = 2.m.(2πζ)/(ρ.D2). Note that U/nD is the reduced velocity. Hence the critical galloping wind velocity can be calculated using the above equation with the gradient (dCy/dα) where α is in radians obtained from graphs of Cy versus α. Likewise the natural frequency n of the structure can be adjusted to increase the critical velocity. 778 Structural Engineering Analysis and Design Second Edition As an example, it may be necessary to determine the fundamental natural frequency of a structure so that it should not flexurally gallop at wind speeds less than U = 30m/s with the flow direction at α = 0. Some parameters are ρ = 1.23 kg/m3, D = 0.1m, m = 25kg/m and ζ = 0.015. Ugallop/nD = 2.Sc/(dCy/dα)α=0 Sc = 2.m.(2πζ)/(ρ.D2) = 2 x 25 x (2π x 0.015) / (1.23 x 0.12) = 383 From the above Cy vs α graph for square sections, (dCy/dα)α=0 = 2.7 (Note α calculated in radians!) Hence 2.Sc/(dCy/dα)α=0 = 2 x 383 / 2.7 = 284 Natural frequency for critical wind speed of 30m/s, n = 30 / (284 x 0.1) = 1.05 Hz. Another example involves the flexural galloping susceptibility assessment of a solid Rhendex pile with a submerged depth of 15.8m in a steady stream. Some additional parameters are D = 0.7m, mass = 607.5kg/m, I = 2.2E-3m4, E = 200E9 N/m2, ζ = 0.01 and ρ = 1020kg/m3. Added water mass = 1020 x ¼ π(0.7)2 = 393kg/m. Total mass = 607.5 + 393 = 1000.5 kg/m Effective length of pile adding a fixing length of 6D say = 15.8 + 6 x 0.7 = 20.0m 3.52 EI 1st natural bending frequency = ≈ 0.93Hz 2π mL4 Ugallop/nD = 2.Sc/(dCy/dα)α=0 Sc = 2.m.(2πζ)/(ρ.D2) = 2 x 1000.5 x (2π x 0.01) / (1020 x 0.72) = 0.25 From the above Rhendex section CD and CL vs α graph, we see that dCL/dα is negative for 25° < α < 50° and 82° < α < 98° for which dCy/dα = CD + dCL/dα is 1.2 and 2.4 respectively. Hence 2.Sc/(dCy/dα)25°<α<50° = 2 x 0.25 / 1.2 = 0.42 and 2.Sc/(dCy/dα)82°<α<98° = 2 x 0.25 / 2.4 = 0.24 Thus, U = 0.42 x 0.93 x 0.7 = 0.27 m/s for 25° < α < 50° and U = 0.24 x 0.93 x 0.7 = 0.14 m/s for 82° < α < 98° Another galloping example involves the torsional galloping of a bridge deck based on experimental motion derivatives as opposed to the static derivatives dCy/dα. Consider a bridge deck with the following parameters, I = 540000kgm2, vertical stiffness per unit length k = 21060N/m, torsional damping ratio ζT = 0.007, ρ = 1.2kg/m3 and width of deck B = 18m. Equating the torsional equation of motion to the Scanlan and Tomko moment and denoting the critical condition to be the onset of negative total damping, the following presents the results. 779 Structural Engineering Analysis and Design Second Edition Estimates of amplitude for a square section can be made from the following graph. Galloping can be avoided by changing the cross section, changing the flow direction, increasing the Scruton number or by increasing damping. Galloping is a 1 DOF system whilst classical flutter is a 2 DOF (bending and torsion) system. Galloping differs from vortex shedding in a few ways. Vortex Shedding Caused by instability of the fluid motion Critical stream velocity depends on shape of body, but not damping Amplitude is limited Damping affects amplitude Galloping Caused by motion of structure Critical stream velocity depends on shape of body AND damping Amplitude is not limited Damping has little effect on amplitude BD 49/01 (valid depending on the aerodynamic susceptibility parameter, Pb and satisfying some geometric constraints) states that a bridge will be stable against galloping and stall flutter if the critical wind speed for bending and torsional motion, Vg is greater than wind speed Vwo Vr is the hourly mean wind speed. Vd is the maximum wind gust speed for the relevant maximum span; K1A is a coefficient selected to give an appropriate low probability of occurrence of these severe forms of oscillation. For locations in the UK, K1A = 1.25. Note that a higher value of K1A is appropriate for other climatic regions, eg typically K1A = 1.4 for a tropical cyclone-prone location. The critical galloping and stall flutter wind speed is considered for vertical bending and torsional motion. Vertical motion need be considered only for bridges of types 3, 3A, 4 and 4A as shown before, and only if b < 4d4. The critical velocity for vertical motion is where the reduced velocity is 780 Structural Engineering Analysis and Design Second Edition Note that ρ is the density of air, m is the mass per unit length of the bridge and fB the natural frequency of bridge in bending. Cg is 2.0 for bridges of type 3 and 4 with side overhang greater than 0.7d4 or 1.0 for bridges of type 3, 3A, 4 and 4A with side overhang less than or equal to 0.7d4; d4 is the reference depth of the bridge; δs is the logarithmic decrement of damping. The following values of δs shall be adopted unless appropriate values have been obtained by measurements on bridges similar in construction to that under consideration and supported on bearings of the same type. If the bridge is cable supported the values given shall be factored by 0.75. Torsional motion shall be considered for all bridge types. The critical velocity shall be taken as follows. and but if bridges of type 3, 3A, 4 and 4A have b < 4d4, Vg shall be taken as the lesser of 20fTd4 or 5fTb. Note that fT is the natural frequency in torsion in Hz and b is the total width of bridge. Eurocode 1-2.4:1995 presents rules for galloping as follows. 781 Structural Engineering Analysis and Design Second Edition 782 Structural Engineering Analysis and Design Second Edition 783 Structural Engineering Analysis and Design Second Edition 784 Structural Engineering Analysis and Design Second Edition 785 Structural Engineering Analysis and Design Second Edition 786 Structural Engineering Analysis and Design Second Edition 787 Structural Engineering Analysis and Design Second Edition 5.4.4.2 Across-Flow Direction Classical Flutter (Divergent Amplitude Response) Flutter occurs under combined (coupled) torsional and bending modes, whereby the reactions caused by the torsional vibrations predominate. It occurs when for a particular phase between torsion and bending, vibrational energy is extracted by the structure from the constant flow of air. Flutter is the oscillatory aeroelastic instability that occurs at some airspeed at which energy extracted from the airstream during a period of oscillation is exactly dissipated by the damping of the structure. The aerodynamic damping is a function of the reduced speed which is defined U U flutter reduced speed = fTb where U is the wind speed, fT the torsional frequency and b the width of the bridge. Instability occurs when the wind velocity is greater than the reduced speed AND the aerodynamic damping, A is greater than the structural damping. This results in the critical flutter speed relationship. The motion is divergent in a range of speeds above the critical flutter speed, here given for fT/fB > 1.2 as follows.  f  0.72.m.r  U flutter critical speed = η.1 +  T − 0.5 . .2.π.f B .b 2   f B  π.ρ.b  where η is the bridge profile shape factor, m is the mass/length of bridge, r the radius of gyration, b the effective width of the bridge along the wind direction, ρ the air density. Important for avoiding flutter is the ratio of torsional to bending natural frequencies (fT/fB). This should be as large as possible (about 3). 788 Structural Engineering Analysis and Design Second Edition Experimental based expressions for lift FL and moment FM are presented. 789 Structural Engineering Analysis and Design Second Edition Aerodynamic coefficients Hi* and Ai* for a thin airfoil (i = 1,2,3) and three streamlined box decks (i = 1,2,3,4) are presented as follows. Flutter can be avoided by choosing a suitable section. Increasing damping does not achieve the same improvement as for vortex shedding or galloping. The Tacoma Narrows Suspension Bridge at Washington, which opened on the 1st of July 1940, failed at a wind speed as low as 67km/h due to flutter on the 6th of November 1940. The Tacoma Narrows Bridge consisted of two 126m towers, two 330m side spans, and a 840m main span stiffened with 2.4m deep girders with span/depth of 350 and span/width of 72. The center of the deck was rising and falling vertically by 0.9m and deflecting laterally by 0.61m. Suddenly, the bridge started twisting violently, with the deck appearing to be twisting by almost 45 degrees. At its ultimate, 180m of the main span tore away from the suspenders, the side spans sagged and the towers tilted 3.6m towards each shore. BD 49/01 (valid depending on the aerodynamic susceptibility parameter, Pb and satisfying some geometric constraints) states that a bridge will be stable against classical flutter if the critical wind speed for bending and torsional motion, Vf is greater than wind speed Vwo Vr is the hourly mean wind speed.Vd is the maximum wind gust speed for the relevant maximum span; K1A is a coefficient selected to give an appropriate low probability of occurrence of these severe forms of oscillation. For locations in the UK, K1A = 1.25. Note that a higher value of K1A is appropriate for other climatic regions, eg. typically K1A = 1.4 for a tropical cyclone-prone location. The critical wind speed for classical flutter is where the reduced velocity VRf is 790 Structural Engineering Analysis and Design Second Edition but not less than 2.5. Note that ρ is the density of air, b is the overall width of the bridge deck, m is the mass per unit length of the bridge, fB the natural frequency of bridge in bending, fT the natural frequency of bridge in torsion and r is the polar radius of gyration of the effective bridge cross section at the centre of the main span (polar second moment of mass/mass)0.5. Flutter analysis utilizes complex eigenvalue analysis to determine the combination of airspeed and frequency for which neutrally damped motion is sustained. Three methods of flutter analysis are provided in MSC.NASTRAN SOL 145, the American flutter method (called the K method in MSC.NASTRAN), an efficient K method (called the KE method) for rapid flutter evaluations, and the British flutter method (called the PK method) for more realistic representation of the unsteady aerodynamic influence as frequency-dependent stiffness and damping terms. Complex eigenvalue analysis is used with the K method, and the QR transformation method is used with the KE and PK methods. Eurocode 1-2.4:1995 presents rules for flutter as follows. 791 Structural Engineering Analysis and Design Second Edition 792 Structural Engineering Analysis and Design Second Edition 793 Structural Engineering Analysis and Design Second Edition 5.4.4.2.1 American K-method The basic equation for modal flutter analysis by the K-method is 794 Structural Engineering Analysis and Design Second Edition For the K-method of solution, the aerodynamic term is converted to an equivalent aerodynamic mass 5.4.4.2.2 British PK-method 5.4.4.2.3 KE-method 795 Structural Engineering Analysis and Design Second Edition 5.5 GL, ML Vibration Fatigue Analysis It has been estimated from time to time that 75% of all machine and structural failures have been caused by some form of fatigue. It was once thought that metal becomes brittle under the action of cyclic loads. This has proved to be incorrect. We know now that fatigue failure starts on a microscopic scale as a minute crack or defect in the material. This gradually grows under the action of stress fluctuations because plastic deformations are not completely reversible. The crack proceeds on planes of the greatest tensile stresses. When the crack reduces the effective cross section to a size that cannot sustain the applied load, the component fractures in ductile failure. Fatigue cracks initiate and grow as a result of cyclic plastic deformation. Without plasticity there can be no fatigue failure. All attempts are made to explain how plasticity is taken into account when determining fatigue life from linear elastic finite element analysis. Fatigue is the failure under repeated or otherwise varying load, which never reaches a level sufficient to cause failure in a single application. The phenomenon was discovered by August Wohler between 1852 and 1870. There are two stages to fatigue failure. In stage I (short crack), a short crack growth occurs controlled by the maximum shear stress i.e. the crack occurs at 45 degrees to the direction of the maximum absolute principal stress. In stage II (long crack), a long crack occurs controlled by the maximum absolute principal stress in a direction perpendicular to the maximum absolute principal stress. We shall only concern ourselves with the more important stage II long crack growth. The fatigue analysis is described for MSC.NASTRAN and the fatigue solver MSC.FATIGUE, which is within the pre and post-processor MSC.PATRAN. Fatigue damage would normally initiate at the surface. Hence, it is quite common to skin solid elements with a very thin mesh of shells (of 0.01mm thickness say) to avoid stress resolution problems i.e. the inaccuracies in extrapolating the stress results from the middle of the solid to the surfaces. In order to skin the solid mesh, the thickness of the solid elements is reduced by the small finite thickness of the shell elements, which have the same material property as the solids. A uniaxial fatigue analysis involves two processes: I. The maximum absolute principal stress or strain field generation in the time or frequency domain II. Fatigue analysis by either (a) the stress life S-N (total life = crack initiation + crack propagation) approach relating local elastic stress to fatigue life, (b) the strain life E-N (crack initiation) approach relating local strain to fatigue life, or (c) the crack propagation method LEFM relating the stress intensity to the crack propagation rate The FE analysis techniques that can be used for the different life prediction methods are as follows. Total Life Pseudo-static Transient Modal Transient Random Frequency Crack Initiation Pseudo-static Transient Modal Transient Crack Growth Pseudo-static Transient Modal Transient Multi-axial fatigue analysis is more complicated and specialist material should be sought. 796 Structural Engineering Analysis and Design Second Edition 5.5.1 Maximum Absolute Principal Stress or Strain Field Generation in the Time or Frequency Domain 5.5.1.1 Choice of Analysis Method There are 4 methods by which the stress or strain field can be generated. I. II. III. IV. The pseudo-static method SOL 101 is used only when the cyclic loading does not induce any dynamic effects in the response of the structure. The transient method SOL 109 can be used where dynamic effects are important on deterministic loadings. The modal superposition transient method SOL 112 performs the FE analysis on deterministic loadings in the modal coordinates instead of the physical coordinates and hence is far more efficient than the transient method. However, sufficient modes must be included. Finally, the frequency domain random analysis (employing SOL 108 or SOL 111) approach may be used very efficiently if the loading is (narrowband or broadband) random, not deterministic like a sine wave or a discernible spike. The results of the fatigue analysis are usually requested at the nodes, not the elements. 797 Structural Engineering Analysis and Design Second Edition 5.5.1.2 GL, ML Pseudo-Static Analysis The analysis procedure is described as follows: (i) (ii) (iii) (iv) Ensure that the maximum frequency of excitation is less than 1/3 of the first fundamental natural frequency of the structure to justify ignoring dynamic effects The maximum frequency of excitation is obtained from an FFT or PSD analysis of the input time history whilst the first fundamental natural frequency of the structure is ascertained from a linear natural modes (SOL 103) analysis. The low frequency of the excitation relative to the lowest natural frequency would ensure that dynamic effects (dynamic amplification) do not contribute significantly to the response of the structure to the cyclic loadings. Hence a pseudo-static based fatigue analysis would be valid. Perform a linear static analysis (SOL 101) with unit static loads at all DOFs with the cyclic loading, each unit load in a separate subcase requesting the element static stress or strain recovery Element static stress or strain recovery is requested for each subcase for all elements in the element coordinate system by specifying the STRESS (PLOT) or STRAIN (PLOT) command. Perform a rotation of the nodal static stress or strain tensors from the element coordinate system to the basic coordinate system and subsequently derive the maximum absolute static principal stress or strain The static stress or strain tensors are requested in the element coordinate system for each and every element in MSC.NASTRAN. The state of static stress or strain of any element must be resolved onto its principal plane to obtain the principal stresses or strains. In general, for a shell element, there will be 2 principal stress or strain tensors whilst a solid element will produce 3 principal stress or strain tensors. For uniaxial fatigue analysis theory to be valid, the minimum absolute principal stresses or strains (σ2, ε2 for shells and σ2, ε2 and σ3, ε3 for solids) be it tensile (extension) or compressive (contraction) must be zero or negligible. This is because the cyclic variation of the minimum absolute principal stresses or strains is not accounted for within the uniaxial fatigue analysis. Another assumption made is that there is negligible rotation of the principal stress or strain plane of each element throughout the variation of the cyclic loadings. In other words, the direction of the maximum absolute principal stress or strain stays approximately constant throughout the loading history. Both of these assumptions are usually valid because in most parts of most structures, the direction of the maximum absolute principal stress or strain is usually constant and the minimum absolute principal stresses or strains are usually negligible. This occurs due to the inherent dominant load path within any part of the structure as a consequence of its geometry. MSC.NASTRAN solves for displacements at the nodes from which the element stress or strain recovery is performed to obtain the element stresses or strains in the corresponding element coordinate system. These stresses or strains are then extrapolated to the nodes in the element coordinate system and are output in the .op2 file. MSC.FATIGUE is employed to transform these nodal stress or strain results into the basic coordinate system. Then, the maximum absolute principal stress or strain is calculated at each node within MSC.FATIGUE. Multiply the unit load static element principal stress fields by their corresponding time histories to obtain the element maximum absolute principal stress field variation in the time domain 798 Structural Engineering Analysis and Design Second Edition 5.5.1.3 GL, ML Transient Analysis The analysis procedure is described as follows: (i) (ii) (iii) Determine the maximum frequency of excitation and the first fundamental natural frequency of the structure to ascertain if dynamic effects are significant Perform a linear transient analysis (SOL 109 or SOL112) with the actual cyclic time signals at the relevant DOFs as input in MSC.NASTRAN within one subcase, requesting the element time domain stress or strain recovery Element time domain stress or strain recovery is requested for all elements in the element coordinate system by specifying the STRESS (PLOT) or STRAIN (PLOT) command. Perform a rotation of the nodal time domain stress or strain tensors from the element coordinate system to the basic coordinate system and subsequently derive the time domain maximum absolute principal stress or strain Two assumptions are made at this stage, first that the state of principal stresses or strains are uniaxial, i.e. the cyclic variation of the minimum absolute principal stresses or strains are insignificant in causing fatigue and secondly that there is negligible rotation of the principal stress or strain plane of each element throughout the variation of the cyclic loadings. These assumptions are usually justified due to the inherent dominant load path within any part of the structure as a consequence of its geometry. MSC.NASTRAN solves for displacements at the nodes from which the element stress or strain recovery is performed to obtain the element stresses or strains in the corresponding element coordinate system. These stresses or strains are then extrapolated to the nodes in the element coordinate system and are output in the .op2 file. MSC.FATIGUE is employed to transform these nodal stress or strain results into the basic coordinate system. Then, the maximum absolute principal stress or strain is calculated at each node within MSC.FATIGUE. 799 Structural Engineering Analysis and Design Second Edition 5.5.1.4 GL, ML Modal Superposition Transient Analysis The analysis procedure is described as follows: (i) (ii) Determine the maximum frequency of excitation and the first fundamental natural frequency of the structure to ascertain if dynamic effects are significant Perform an eigenvalue analysis requesting modal nodal stress or strain recovery within a linear modal transient analysis SOL112 with the actual cyclic time signals at the relevant DOFs as input in MSC.NASTRAN requesting the time domain modal responses in modal space $ EXECUTIVE CONTROL SECTION SOL 112 $ CASE CONTROL SECTION SUBCASE 1 $ Normal modes analysis to obtain the modal stress or strain field ANALYSIS = MODES METHOD = < ID IN EIGRL > ELSTRESS(PLOT)=ALL STRAIN(PLOT)=ALL $ SUBCASE 2 $ Modal transient response to obtain the modal responses in modal space METHOD = < ID IN EIGRL > DLOAD = < ID OF TLOAD1 > SDISPLACEMENT(PUNCH,PLOT) = ALL For each mode, there is a modal response (in modal space) at all DOFs as a function of time. These can be viewed in the punch file requested if intended. (iii) From the nodal time domain stress or strain tensors in the basic coordinate system derive the time domain maximum absolute principal stress or strain Two assumptions are made at this stage, first that the state of principal stresses or strains are uniaxial, i.e. the cyclic variation of the minimum absolute principal stresses or strains are insignificant in causing fatigue and secondly that there is negligible rotation of the principal stress or strain plane of each element throughout the variation of the cyclic loadings. These assumptions are usually justified due to the inherent dominant load path within any part of the structure as a consequence of its geometry. Since this is a modal approach, MSC.NASTRAN solves for modal displacements at the nodes from which the modal nodal stresses or strains are computed in the basic coordinate system and stored in the .op2 file. Hence, MSC.FATIGUE does not need to be employed to transform these nodal stress or strain results into the basic coordinate system as this has already been done. Then, the maximum absolute principal stress or strain is calculated at each node within MSC.FATIGUE by multiplying the modal responses (in modal space) to the mode shapes. 800 Structural Engineering Analysis and Design Second Edition 5.5.1.5 GL, ML Frequency Domain Stationary (and Ergodic) Random Analysis The analysis procedure is described as follows: (i) (ii) (iii) (iv) (v) Determine the maximum frequency of excitation and the first fundamental natural frequency of the structure to ascertain if dynamic effects are significant Calculate the input PSDs and CPSDs corresponding each and every loaded DOF from the time signals and generate the 3x3 PSD matrix The PSD matrix is 3x3 to correspond to loadings in the three basic (global) directions. Perform a linear frequency response analysis (SOL 108 or SOL 111) with unit harmonic loads at all the corresponding loaded DOFs as input in MSC.NASTRAN within one subcase, requesting the nodal stress or strain transfer function Nodal stress or strain transfer functions are requested by specifying the STRESS (PLOT) or STRAIN (PLOT) command. If the modal approach SOL 111 is employed, request the utilization of modes up to at least 3 times the highest loading frequency. It is important to choose the points of the transfer function to include points that define the natural modes of the structure well, and also those that fall in the vicinity of points that define the prominent parts of the input PSD. From the nodal frequency domain stress or strain transfer function in the basic coordinate system derive the maximum absolute principal stress or strain transfer functions Two assumptions are made at this stage, first that the state of principal stresses or strains are uniaxial, i.e. the cyclic variation of the minimum absolute principal stresses or strains are insignificant in causing fatigue and secondly that there is negligible rotation of the principal stress or strain plane of each element throughout the variation of the cyclic loadings. These assumptions are usually justified due to the inherent dominant load path within any part of the structure as a consequence of its geometry. In the frequency domain, MSC.NASTRAN solves for nodal stress or strain transfer function in the basic coordinate system. Hence, MSC.FATIGUE does not need to be employed to transform these nodal stress or strain transfer function into the basic coordinate system as this has already been done. However, the maximum absolute principal stress or strain transfer function is calculated at each node within MSC.FATIGUE. Multiply the input PSD matrix to the transfer function squared to obtain the response maximum absolute principal stress or strain PSD 801 Structural Engineering Analysis and Design Second Edition 5.5.2 Stress-Life (S-N), Strain-Life (E-N) or Crack Propagation LEFM Uniaxial Fatigue Analysis The S-N (total life = crack initiation + crack propagation) method is appropriate for long life (high-cycle) fatigue problems where there is little plasticity as the method is based on nominal stresses. The S-N method does not work well when strains have a significant plastic component, as S is the elastic stress range. Fatigue life of N greater than 104-105 (high-cycle fatigue) can be analyzed with the S-N method. The S-N method is not suitable for components where crack initiation or crack growth modelling is not appropriate, e.g., composites, welds, plastics, and other non-ferrous materials. The S-N method does not account for the sequence of loading, obviously higher stress ranges early in the life is more detrimental than later. S-N method is especially appropriate if large amounts of S-N material data exist. On the other end of the spectrum of design philosophies is that of fail safe. This is where a failure must be avoided at all costs. And if the structure were to fail it must fall into a state such that it would survive until repairs could be made. This is illustrated with a stool having six legs. If one leg were to fail, the stool would remain standing until repairs could be made. This philosophy is heavily used in safety critical items such as in the aerospace or offshore industries. The E-N (crack initiation) method is appropriate for fatigue life of N less than 104-105 (low-cycle fatigue). It can also be used for long life (high-cycle) fatigue problems. The E-N method is appropriate for most defect free metallic structures and components where crack initiation is important. It is appropriate for components that are made from metallic, isotropic ductile materials which have symmetric cyclic stress-strain behavior. The safe life philosophy is a philosophy adopted by many, but especially the ground vehicle industry. Products are designed to survive a specific design life. Full scale tests are usually carried out with margins of safety applied. In general, this philosophy results in fairly optimized structures such as a stool with three legs. Any less than three legs and it would fall over. This philosophy adopts the crack initiation method and is used on parts and components that are relatively easy and inexpensive to replace and not life threatening if failure were to occur. Most of the life is taken up in the initiation of a crack. The propagation of that crack is very rapid and short in comparison. The crack propagation method is appropriate for pre-cracked structures or structures which must be presumed to be already cracked when manufactured such as welds. It is useful for pre-prediction of test programs to avoid testing components where cracks will not grow and for the planning inspection programs to ensure checks are carried out with the correct frequency. It is beneficial to simply determine the amount of life left after crack initiation. Again it is appropriate only for components that are made from metallic, isotropic ductile materials which have symmetric cyclic stress-strain behavior. The middle ground philosophy is that of damage tolerance. This philosophy, adopted heavily in the aerospace community and nuclear power generation, relies on the assumption that a flaw already exists and that a periodic inspection schedule will be set up to ensure that the crack does not propagate to a critical state between inspection periods. As implied, this philosophy adopts the crack growth method. This is illustrated using our stool (now with four legs) but with someone inspecting it. This particular design philosophy is generally used in conjunction with the fail safe philosophy, first to design for no failure, and then to assume that, for whatever reason, a flaw exists and must be monitored. 802 Structural Engineering Analysis and Design Second Edition 5.5.2.1 Stress-Life (S-N) (Total Life) Uniaxial Fatigue Analysis Stress life (S-N) prediction is appropriate for high endurance fatigue, i.e. fatigue failures that occur from about 104-105 cycles to infinity. On a double logarithmic plot logS vs logN, most steels and ferrous alloys exhibit a horizontal line below which the metal cannot be fractured by fatigue, known as the fatigue or endurance limit. For ferrous alloys with strength below 1400MPa, the endurance limit is approximately half its ultimate strength. The endurance limit for ferrous alloys with an ultimate strength above 1400MPa is approximately 700MPa, i.e. that is the limitation. In addition to this, the stress at 103 cycles, S3, can be approximated by 0.9Su. Using the Goodman relationship (for mean tensile stress correction) and knowing the endurance limit, it can be quickly ascertained if fatigue would be an issue or not. Unlike steel, aluminium does not show an endurance limit. S refers to the stress range whilst N refers to the number of cycles to failure. The S-N curve should always be quoted with the corresponding probability of failure, 0% and 50%. Knowing just the 50% probability of failure S-N curve is meaningless as there is no information of the scatter of results. The S-N curve should correspond to the material M-S-N and not the component, the latter of which is usually referred to as the C-S-N curve. Unlike the CS-N curve, the M-S-N curve is independent of the test specimen. Only 2 parameters are required to define the M-SN curve, namely m and k. Usually the double logarithmic curve is used and so the log S versus log N plots straight lines. Log S NSm = K Sut hence, log N + m log S = log K 1 1 log S = − log N + log K m m Low Cycle High Cycle 103-104 Log N 106-107 As mentioned, fatigue cannot occur without some local plasticity. The S-N method makes no effort to define the amount of plasticity or compensate for it in any specific manner. All plasticity is built into the S-N curve itself. Part features that produce stress concentrations greatly reduce the fatigue life. The stress concentration factor is Kt (geometry based). In the FE model, Kt = 1 if the stress concentrations is due to a geometry such as a hole that is explicitly modeled. Otherwise, a non-unity value of Kt should be applied. 803 Structural Engineering Analysis and Design Second Edition The fatigue concentration factor is Kf (material based). This is similar to the stress concentration, Kt, except it accounts for the fact that small notches have less effect on fatigue than is indicated by Kt. This has led to the idea of a fatigue concentration factor, Kf, which is normally less than Kt, being introduced and being used to replace Kt. Kf is related to Kt according to where p’ is a material constant dependent on grain size and strength and r is the notch root radius. The presence of residual compressive stresses on the surface if a metal has been shown to be a very successful method of improving fatigue endurance. On the other hand, the presence of residual tensile stresses on the surface has a very detrimental effect. Other factors that affect fatigue life worth bearing in mind are temperature effects, corrosion and surface finish and conditioning. Tests on a number of aluminium or steel alloys ranging down to – 50 degrees have shown little affect on the fatigue life. On the other hand, at temperature in excess of 400 degrees, there is a rapid fall in fatigue strength. Corrosion lowers fatigue life considerably. Corrosion is a process of oxidation, and under static conditions a protective oxide film is formed which tends to retard further corrosion. However, with cyclic loading, the protective coating is ruptured in every cycle allowing further corrosion. The combined effects of corrosion and fatigue can be quite detrimental. Fatigue failures in metals almost always develop at a free surface. Hence the surface finish and conditioning has a significant effect on the fatigue life. A polished surface finish is much better than a rough machined surface since this reduces the mild stress concentrations at the surface. The hardening conditioning processes increase fatigue strength whilst plating and corrosion protection tends to diminish fatigue strength. In TIME DOMAIN solutions, the static response must be added to the dynamic response if the dynamic analysis is performed about the initial undeflected (by the static loads) state with only the dynamic loads applied, hence causing the dynamic response to be measured relative to the static equilibrium position. Hence, the total response = the dynamic response + the static response to static loads. Alternatively, in TIME DOMAIN solutions, if the dynamic analysis is performed with the deflected static shape as initial input and the static loads maintained throughout the dynamic excitations, the total or absolute response (static and dynamic) is obtained straight away from the dynamic analysis. Hence total response = dynamic response (which already includes the static response to static loads). Either way, the mean of the response must be ascertained in order to perform mean stress correction. The time domain (including the pseudo-static) fatigue analysis is summarized as follows: (i) Perform rainflow cycle counting (Matsuishi and Endo) on the irregular sequence yielding the stress range S, number of cycles n over the duration of the time signal (hence n in Hertz or cycles per second), and the mean for each bin. (ii) Perform mean (tensile) stress correction on the stress range of each bin using the Goodman straight line, the Gerber parabola or Soderberg straight line on plots of stress amplitude versus mean stress. 804 Structural Engineering Analysis and Design Second Edition Gerber is the upper bound whilst Goodman is the lower bound. Goodman is the most commonly employed. Soderberg is a more conservative line for design purposes using a yield stress Sy instead of the tensile strength Su in the Goodman relationship. It can be concluded that an increase in tensile mean stress in the cycle reduces the allowable range of stress. Compressive mean stress appear to cause little or no reduction in stress range and some materials even show an increase. Hence, it is also usual to assume no mean stress correction for compressive stresses as a conservative approximation as compression aids in protecting against fatigue failure. σ a = stress amplitude σ m = mean stress S u = ultimate tensile strength S e = equivalent stress for σ m = 0 Graphically this looks like the plot below, at least for Goodman, if you draw a line connecting Su to the intersection of σa and σm and then continue it on to the stress amplitude axis, this will indicate the equivalent stress Se with zero mean. This stress is then used to look up damage on the S-N curve using the Palmgren-Miners rule. The method employed for mean stress correction is usually Goodman. This relation is good for fracture fatigue. If yield is to be used as the failure criterion, the Soderberg relation which replaces Su with the tensile yield Sy is used. (iii) Employ the Palmgren-Miners rule and the constant amplitude fully reversed (i.e. zero-mean as mean stress correction already accounted for by Goodman, Gerber or Soderberg) S-N curve to estimate the damage and hence life (reciprocal of damage). The Palmgren-Miner hypothesis suffers from the fact that it does not take the sequence of loading into account. Obviously larger stress ranges early in the life of the structure would be more detrimental than later. Failure occurs when Damage = n ∑ N = 1.0 The units of n is Hz or cycles per second. N is in cycles. Hence damage as calculated from the Palmgren-Miner equation will be in per seconds. Thus, the life, which is the reciprocal of damage, will be in seconds. In FREQUENCY DOMAIN solutions, not only that the static response has to be added separately, but also the mean of the dynamic excitation has also got to be added separately as a static response. This is because the mean of the dynamically applied force is not included in the dynamic excitations. Hence the total response in this frequency domain dynamic analysis = static response to mean of dynamic excitation + dynamic response + static response to static loads. The mean response thus has to be identified from the fluctuating response. 805 Structural Engineering Analysis and Design Second Edition The frequency domain random fatigue analysis is summarized as follows: (i) Perform equivalent rainflow cycle counting (to generate the PDF) on the response PSD. The intensity of the signal is given by the RMS. The number of cycles per second is given by the number of peaks per second, E[P] (peaks/s), function of the moments of the PSD. The total number of cycles, St is S t = E[P].T Hence the number of cycles for a particular stress range is the probability (from the integral of the PDF) multiplied by the total number of cycles number of cycles = (p(S).dS).S t Thus, the number of cycles per second for the particular stress range, ni is given by n i = (p(S).dS).S t / T = (p(S).dS).E[P] The frequency content or bandedness (in effect the distribution of cycles) of the random PSD needs to be quantified in order to choose and justify the correct method of generating the PDF. This can be done by calculating irregularity factor, γ or by the Dirlik rainflow cycle distribution, both of which is a function of four moments of the PSD namely m0, m1, m2 and m4. Performing a frequency domain random analysis on a deterministic (as opposed to narrowband or broadband random) signal is very conservative. For instance, the PSD of a sine wave with an amplitude of say 140MPa is simply a spike. We know that the RMS of the sinusoidal time signal is 0.7071 times the amplitude, hence 100MPa. This RMS will be represented by the area of the PSD. We also know that generating a random time signal from a PSD will predict a peak amplitude of 3 (to 4.5) times the RMS, hence 300MPa here. This is because the amplitude distribution of a narrow or broadband signal is Gaussian. This is much higher than the 140MPa value of the original signal. Thus the frequency domain approach will be conservative as the greatest damage in a fatigue analysis will be produced by the large stress ranges even with a relatively low number of cycles. If we have a narrowband process, all we really need is the RMS to perform a fatigue calculation. The narrowband solution is traditionally the method employed to ascertain the distribution of the cycles. J.S. Bendat (1964) developed the theoretical basis for the so called Narrow Band solution. However, the fact that this solution was suitable only for a specific class of response conditions was an unhelpful limitation for the practical engineer. This was the first frequency domain method for predicting fatigue damage from PSDs and it assumes that the PDF of peaks is equal to the PDF of stress amplitudes. The Narrow Band solution was then obtained by substituting the Rayleigh PDF of peaks with the PDF of stress ranges. The fact that the fatigue PDF is stress range and the Rayleigh PDF is the peak is accounted for. The Rayleigh is actually only a function of the RMS and hence just of m0 as RMS = √m0. The narrowband solution is however very conservative (approximately by 100 times) for broadband processes as it assumes that all positive peaks are matched with corresponding troughs of similar 806 Structural Engineering Analysis and Design Second Edition magnitude. The problem with this solution is that by using the Rayleigh PDF, positive troughs and negative peaks are ignored and all positive peaks are matched with corresponding troughs of similar magnitude regardless of whether they actually form stress cycles. For wide band response data the method therefore overestimates the probability of large stress ranges and so any damage calculated will tend to be conservative. This is illustrated below. The above figure shows two time histories. The narrow band history is made up by summing two independent sine waves at relatively close frequencies, while the wide band history uses two sine waves with relatively widely spaced frequencies. Narrow banded time histories are characterized by the frequency modulation known as the beat effect. Wide band processes are characterized by the presence of positive troughs and negative peaks and these are clearly seen in the overhead as a sinusoidal ripple superimposed on a larger, dominant sine wave. The problem with the narrow band solution is that positive troughs and negative peaks are ignored and all positive peaks are matched with corresponding troughs of similar magnitude regardless of whether they actually form stress cycles. To illustrate why the narrow band solution becomes conservative with wide band histories, take every peak (and trough) and make a cycle with it by joining it to an imaginary trough (peak) at an equal distance the other side of the mean level. This is shown in the bottom graph. It is easy to see that the resultant stress signal contains far more high stress range cycles than were present in the original signal. This is the reason why the narrow band solution is so conservative. For broadband signals, Dirlik has produced an empirical closed form expression for the PDF of rainflow ranges, which was obtained using extensive computer simulations to model the signals using the Monte Carlo technique. This equation has been found to be a widely applicable solution which consistently out performs all of the other available methods. 807 Structural Engineering Analysis and Design Second Edition Since Bendat first derived the narrow band solution a number of methods have been derived in order to improve on its short comings. Tunna and Wirsching solutions are both, effectively, corrected versions of the narrow band approach. Tunna’s equation was developed with specific reference to the railway industry. Wirsching’s technique was developed with reference to the offshore industry, although it has been found to be applicable to a wider class of industrial problems. The Chaudhury and Dover, and Hancock solutions were both developed for the offshore industry. They are both in the form of an equivalent stress parameter. Neither tend to work well when used for other industrial problems. Furthermore, the omission of rainflow cycles from the solution output for both approaches is a further limitation. The Steinberg solution method is used by the electronics industry in the USA. 808 Structural Engineering Analysis and Design Second Edition The approach of Steinberg leads to a very simple solution based on the assumption that no stress cycles occur with ranges greater than 6 rms values. The distribution of stress ranges is then arbitrarily specified to follow a Gaussian distribution. Note that the PDF predicts 68.3% time at 2 rms, 27.1% time at 4 rms, and 4.3% time at 6 rms. It is possible to define the maximum stress range used in the subsequent fatigue analysis. If this is set at 6 rms it is possible to see that large stress ranges are omitted using this approach. MSC.FATIGUE will set this value automatically, if not over ridden, to be somewhere around 9 rms for stress range! Anything less than this is likely to result in an under prediction of fatigue damage. Of course this is counter balanced by the fact that medium range stress cycles of levels between 4 and 6 rms are over predicted. Nevertheless it must be stated that this approach is very questionable. It is included only as a means of allowing designers in the electronics industry, who are used to the Steinberg approach, a means of comparison. (ii) Mean (tensile) stress correction cannot be accounted with the PSD method as the PSD contains not any mean. (iii) Employ the Palmgren-Miners rule. Failure occurs when ni Damage = = 1.0 N(Si ) Employing the S-N curve, K N(S i ) = m S the damage, D is calculated as follows ni Damage, D = N(S i ) ∑ ∑ = E[P] m S p(S)dS K ∫ 809 Structural Engineering Analysis and Design Second Edition The units of n is Hz or cycles per second. N is in cycles. Hence damage as calculated from the Palmgren-Miner equation will be in per seconds. Thus, the life, which is the reciprocal of damage, will be in seconds. A good method to check whether a PSD has been specified correctly from a time signal is to perform a fatigue analysis with the PSD as the response PSD in the frequency domain, doing the equivalent rainflow count (with the Dirlik algorithm) and comparing the stress-life results with a fatigue analysis in the time domain with the time signal. The rainflow count can also be compared. This checking method will verify that the time signal is random, Gaussian and stationary. Alternatively, as done usually for any random analysis, the PSD can be converted back into the time signal and the statistics of the new signal compared with that of the original signal. An example of a hand-based random frequency domain fatigue analysis is presented. Consider a typical steel SN curve. The idealized response stress PSD is as follows. The statistics of the PSD are derived. Two hand methods can be used to approximate the frequency domain random fatigue analysis. One is used when the PSD is narrowbanded and the other used when the PSD is broadbanded. For a narrowband approximation, an equivalent solitary sinusoidal wave is derived from the RMS, i.e. 810 Structural Engineering Analysis and Design Second Edition Equivalent Sinusoidal Wave Range = √2 x 112 x 2 = 315 MPa. Hence, D= n E[P] ∑ N =  3728  1 / 0.238 =    S  9.807  3728     315  1 / 0.238 = 9.807 cycles / s 32292.2 cycles = 3.04 x10 − 4 per second Thus, the life which is the reciprocal is 3293s or 0.92 hours. For a broadbanded approximation, Equivalent 1Hz Sinusoidal Wave Range = √2 x √10000 x 2 = 283 MPa. Equivalent 10Hz Sinusoidal Wave Range = √2 x √2500 x 2 = 141 MPa. Hence, noting that n corresponds to the frequency of the waves, namely 1Hz and 10Hz, n 1 Hz 10 Hz D= = + = 1.9743x10 −5 + 1.0571x10 −5 1 / 0.238 N  3728 1 / 0.238  3728  cycles  cycles     283   141  ∑ = 3.0314 x10 −5 per second Thus the life is 32987s or 9.2 hours. The broadbanded approximation is better since the 1Hz and 10Hz is well separated. Note that the foregoing two hand approximations of the PSD with deterministic signals is not necessarily conservative or unconservative, but simply approximations. Contrast with the aforementioned fact that representing a deterministic signal with a PSD and performing a narrowband or broadband solution is conservative, and also performing a narrowband solution on a broadband PSD is also conservative. With the rigorous computational method, using the damage expression ni Damage, D = N(S i ) ∑ E[P].T m S p(S)dS K the Narrow Band solution gives life of 0.41 hours (cf. hand based 0.92 hours) and the Dirlik gives life of 2.13 hours (cf. hand based 9.2 hours). = ∫ 811 Structural Engineering Analysis and Design Second Edition 5.5.2.2 Strain-Life (E-N) (Crack Initiation) Uniaxial Fatigue Analysis Strain life (E-N) prediction is appropriate for low endurance fatigue, i.e. fatigue failures that occur before 104-105 cycles. Low cycles to failure does not necessarily mean a short design life because the frequency of cyclic loading can be small. For instance, an aircraft fuselage is only pressurized once every flight and so it will take years to accumulate 104-105 cycles. Failure at low endurance results from stresses and strains that are high and will result in marked plastic deformation (hysteresis) in every cycle. Hence, strain-life methods are useful when cycles have some plastic strain component. The E-N curves are related to the plastic strain range εp. This is also the width of the hysteresis loop. The E-N relationship of the following form applies for most metals up to 105 cycles. εpNα = k A log εp versus log N graph plots a straight line. The constant α is between 0.5 and 0.6 for most metals at room temperature. 6 parameters are required to fully define the E-N curve. With linear finite element analysis, Neuber’s rule can be employed to account for nonlinear stress strain material curves in the fatigue analysis. The strain-life fatigue analysis can be performed in the time (not frequency) domain. 812 Structural Engineering Analysis and Design Second Edition 5.5.2.3 Crack Propagation LEFM Uniaxial Fatigue Analysis The crack propagation fatigue analysis is more complicated and specialist material should be sought. The crack propagation fatigue analysis can be performed in the time (not frequency) domain 813 Structural Engineering Analysis and Design Second Edition 5.5.3 Stress-Life (S-N), Strain-Life (E-N) or Crack Propagation LEFM Multi-axial Fatigue Analysis Multi-axial fatigue analysis is more complicated and specialist material should be sought. 814 Structural Engineering Analysis and Design Second Edition 5.6 GL, ML Passive Structural Motion Control Methods of passive structural motion control are: i. Optimum stiffness and mass distribution ii. Isolation systems iii. Optimum damping distribution iv. Tuned mass damper systems 5.6.1 Optimum Stiffness and Mass Distribution 5.6.1.1 Concepts of Forced Frequency Response of Deterministic Periodic Harmonic Load Excitations In a modal forced frequency response analysis, the modal response in modal coordinates ξi and the modal response in physical coordinates ui(t) are p p 2ζ i ω / ω ni ξ i (ω) = D i (ω) 0i e − iθi = D i (ω) 2 0i e − iθi , θ i = tan −1 2 Ki ω ni M i 1 − ω 2 / ω ni {u i ( t )} = Re al [{φ i }ξ i (ω)e iω t ( ] ) The relative importance of each mode is encapsulated in the values of the modal responses ξi. However, the physical response effects can be more critical from less significant modes (i.e. with lower modal responses) due to the inherent shape of the eigenvector even if the scaling factor (i.e. the modal response) is smaller. The following parameters are of particular interest in controlling the modal response: I. The modal mass and (the amplitude of the) modal force must be considered together as their magnitudes are related to the arbitrary normalization of φi. MAX normalization scales the eigenvectors such that their maximum component is unity and all other components less than unity. The relative magnitude of the modal mass between different modes scaled by MAX is not in itself an indication of the relative importance of the particular mode as that also depends on the magnitude and location of the applied load excitation, given by the amplitude of the modal force. To reduce the modal response ξi, the modal mass should be maximized AND the amplitude of the modal force should be minimized. The modal mass will be maximized if there is more structural mass in the mode, hence the heavier the structure, the greater shall be the modal mass of most modes, and the lower the modal response. The amplitude of the modal force will be minimized if the amplitude of the applied force is minimized and if the location of the applied force corresponds to the DOF with smaller components of the eigenvector. This is obvious from a physical viewpoint, as clearly the modal response should be greater if the excitation is applied at the maximum locations of the eigenvector. With MAX normalization, the value of the modal mass is still of significance. A graph of (MAX normalized) modal mass versus modal frequency is most illustrative of the global and local modes. The greater the modal mass, the lower will be the response assuming constant amplitude of modal force. A very small modal mass (several orders of magnitude smaller than that of other modes) obtained from MAX normalization indicates a local mode or an isolated mechanism. If the applied force were to be located at the mechanism, the amplitude of the modal force may be significant, and hence so may the modal response. If the distribution of mass is uniform, then higher modes of the same type (for instance higher bending modes relative to the fundamental bending mode) MAY have the same MAX normalized modal masses (simply supported beam modal masses 0.5mL and cantilever beam modal masses 0.25mL). However other types of global modes of higher frequency than the fundamental frequency may have lower modal masses. For instance, the first torsional mode of a tower, which may be of a higher natural frequency than the first bending mode, may have a lower modal mass. This means that higher frequency global modes can also be significantly excited if the applied force was such that it corresponded to the greater values of their eigenvector. 815 Structural Engineering Analysis and Design Second Edition T5 VCR REAL MODAL ANALYSIS - MODAL MASS 250.000 S econdary Tower Bending Modes 225.000 Modal Mass (Tonnes) 200.000 175.000 150.000 Primary Tower Torsion Mode Primary Tower Bending Modes 125.000 100.000 75.000 50.000 Cable Modes Cable Modes Cable Modes Cable Modes 25.000 0.000 0 5 10 15 20 25 30 35 40 45 50 Mode Number Hence, the modal masses of each and every mode are values that can be compared if all the modes had the same amplitude of modal force. The amplitude of the modal force for each and every mode can be made to be the same if there is only one concentrated applied force at one DOF and if the POINT normalization corresponding to that DOF is used for all modes. POINT normalization allows the user to choose a specific DOF at which the modal displacements are set to 1 or –1. Hence, the amplitude of the modal force for all modes will be the same and only the modal mass need to be compared. In this case, there will be significant difference in the order of magnitude of different global modes. The higher the modal mass with this method, the lower shall be the modal response. However, this normalization is not recommended because for complex structures, the chosen component may have very small values of displacement for higher modes causing larger numbers to be normalized by a small number, resulting in possible numerical roundoff errors and ridiculously higher modal masses. For instance, if the POINT normalization points to a DOF component which does not really exist in a particular mode, than all the other eigenvector terms will be normalized by a very small number, which will certainly result in numerical errors. For ANY natural mode, the (magnitude of the) dynamic amplification factor, Di(ω) becomes infinite or is limited only by the modal damping of the particular mode when the excitation frequency approaches the natural frequency of the mode. The higher the modal damping, the lower the (magnitude of the) modal dynamic amplification factor, Di(ω). Hence, the modal amplification can be reduced by either mistuning the frequencies of excitation and the modal natural frequencies or by increasing the modal damping. Dimax occurs when ω/ωn = (1-2ζ2)1/2. Variation of D with Frequency Ratio For Diffe rent Damping Dynamic Amplification Factor, D II. 6 5 4 zhi=0 zhi=0.1 D i (ω) = zhi=0.2 3 2 1 0 zhi=1 zhi=2 0 1 2 Frequency Ratio ω / ω n 816 D i max = (1 − ω ( 1 2 / ω ni 1 2ζ 1 − ζ 2 ) ) 2 2 + (2ζ i ω / ω ni ) ; 2 Structural Engineering Analysis and Design Second Edition III. Higher modes are less significant then lower modes because of the higher natural frequency ωni2 in the expression for the modal response ξi. Hence, in order to reduce the total steady-state response (by controlling the distribution of mass, stiffness and damping) to a fixed frequency and amplitude of excitation, the following may be undertaken. I. The structural mass distribution, stiffness distribution and boundary conditions are modified so that there are no natural frequencies close to the frequency of excitation (and causing resonance) in order to minimize the (magnitude of the) dynamic amplification factor, Di(ω). If the lowest natural frequency can be made significantly greater than the excitation frequency, then all the natural modes respond in a quasi-static manner to the excitation, and thus the response will only be dependent upon the amplitude of excitation as the frequency is low enough to be considered static. If this cannot be done, the natural modes should be tuned such that the excitation frequency is much greater than the lower natural frequencies. The response of the lower modes will be governed by inertial forces (the response of which is even lower than the quasi-static response) and the (magnitude of the) dynamic amplification factor, Di(ω) will be minimized. However, Di(ω) of higher modes will be more significant. But since ωni2 features in the denominator of the modal response expression ξi, the higher modes will produce a lower modal response (although the modal physical response could be significant) when resonated. II. The mass distribution of the structure is increased in order to increase the modal masses (specifically of the modes with significant modal response ξi, but generally all), which in turn reduces the modal response ξi. This however will lower the natural frequencies and will affect the (magnitude of the) dynamic amplification factor, Di(ω) of I. III. The stiffness distribution of the structure is increased in order to increase the natural frequencies ωni2 (specifically of the modes with significant modal response ξi, but generally all), which feature in the denominator of the modal response ξi expression. This will however affect the (magnitude of the) dynamic amplification factor, Di(ω) of I. IV. The boundary conditions of the structure are altered in order to increase the natural frequencies ωni2 (specifically of the modes with significant modal response ξi, but generally all), which feature in the denominator of the modal response ξi expression. This will however affect the (magnitude of the) dynamic amplification factor, Di(ω) of I. V. The location and direction of the applied load excitation is modified to not correspond to the large locations of the modes with significant modal response ξi in order to reduce the amplitude of the modal force, which in turn will reduce the modal response ξi. VI. The damping distribution is modified such as to maximize the modal damping of the modes with significant modal response ξi. This is done in order to minimize the (magnitude of the) dynamic amplification factor, Di(ω) and hence minimizing the modal response ξi. If resonance is unavoidable, damping should be incorporated, as it is most efficient at resonance. For the design of explicit dampers, it is necessary to find the location and range of the damping parameter for optimum damping of a particular mode. The optimum location will clearly be at the position of the maximum components of the eigenvector. Optimum values of the viscous damping coefficient c (Ns/m) depend on the optimum modal damping obtained for a particular range of damping constant. There is always a plateau where the values of the damping constant c will give the optimum (highest) modal damping. This plateau range is obtained computationally by running repetitive complex modal analysis (MSC.NASTRAN SOL 107) with varying damping constants, and observing the range which gives the optimum damping for the structural mode that is to be damped. 817 Structural Engineering Analysis and Design Second Edition 5.6.1.2 Concepts of Forced Transient Response of Deterministic Load Excitations In a modal forced transient response analysis, the modal response in modal coordinates ξi and the modal response in physical coordinates ui(t) are p p ξ i ( t ) = D i ( t ) 0i = D i ( t ) 2 0i Ki ω ni M i {u i ( t )} = {φ i }ξ i ( t ) The relative importance of each mode is encapsulated in the values of the modal responses ξi. However, the physical response effects can be more critical from less significant modes (i.e. with lower modal responses) due to the inherent shape of the eigenvector even if the scaling factor (i.e. the modal response) is smaller. The following parameters are of particular interest in controlling the modal response: I. The modal mass and (the amplitude of the) modal force must be considered together as their magnitudes are related to the arbitrary normalization of φi. MAX normalization scales the eigenvectors such that their maximum component is unity and all other components less than unity. The relative magnitude of the modal mass between different modes scaled by MAX is not in itself an indication of the relative importance of the particular mode as that also depends on the magnitude and location of the applied load excitation, given by the amplitude of the modal force. To reduce the modal response ξi, the modal mass should be maximized AND the amplitude of the modal force should be minimized. The modal mass will be maximized if there is more structural mass in the mode, hence the heavier the structure, the greater shall be the modal mass of most modes, and the lower the modal response. The amplitude of the modal force will be minimized if the amplitude of the applied force is minimized and if the location of the applied force corresponds to the DOF with smaller components of the eigenvector. This is obvious from a physical viewpoint, as clearly the modal response should be greater if the excitation is applied at the maximum locations of the eigenvector. With MAX normalization, the value of the modal mass is still of significance. A graph of (MAX normalized) modal mass versus modal frequency is most illustrative of the global and local modes. The greater the modal mass, the lower will be the response assuming constant amplitude of the modal force. A very small modal mass (several orders of magnitude smaller than that of other modes) obtained from MAX normalization indicates a local mode or an isolated mechanism. If the applied force were to be located at the mechanism, the amplitude of the modal force may be significant, and hence so may the modal response. If the distribution of mass is uniform, then higher modes of the same type (for instance higher bending modes relative to the fundamental bending mode) MAY have the same MAX normalized modal masses (simply supported beam modal masses 0.5mL and cantilever beam modal masses 0.25mL). However other types of global modes of higher frequency than the fundamental frequency may have lower modal masses. For instance, the first torsional mode of a tower, which may be of a higher natural frequency than the first bending mode, may have a lower modal mass. This means that higher frequency global modes can also be significantly excited if the applied force was such that it corresponded to the greater values of their eigenvector. 818 Structural Engineering Analysis and Design Second Edition T5 VCR REAL MODAL ANALYSIS - MODAL MASS 250.000 S econdary Tower Bending Modes 225.000 Modal Mass (Tonnes) 200.000 175.000 150.000 Primary Tower Torsion Mode Primary Tower Bending Modes 125.000 100.000 75.000 50.000 Cable Modes Cable Modes Cable Modes Cable Modes 25.000 0.000 0 5 10 15 20 25 30 35 40 45 50 Mode Number Hence, the modal masses of each and every mode are values that can be compared if all the modes had the same amplitude of modal force. The amplitude of the modal force for each and every mode can be made to be the same if there is only one concentrated applied force at one DOF and if the POINT normalization corresponding to that DOF is used for all modes. POINT normalization allows the user to choose a specific DOF at which the modal displacements are set to 1 or –1. Hence, the amplitude of the modal force for all modes will be the same and only the modal mass need to be compared. In this case, there will be significant difference in the order of magnitude of different global modes. The higher the modal mass with this method, the lower shall be the modal response. However, this normalization is not recommended because for complex structures, the chosen component may have very small values of displacement for higher modes causing larger numbers to be normalized by a small number, resulting in possible numerical roundoff errors and ridiculously higher modal masses. For instance, if the POINT normalization points to a DOF component which does not really exist in a particular mode, than all the other eigenvector terms will be normalized by a very small number, which will certainly result in numerical errors. In general, Di(t) is a function of the natural circular frequency ωni2 = Ki/Mi or the damped natural circular frequency ωd, the time duration of loading td and the general time t. For a SDOF system, Dimax can be found by differentiation and is a function of the natural circular frequency ωni2 = Ki/Mi or the damped natural circular frequency ωd and the time duration of loading td. A graph of Dimax versus td / Ti is extremely illustrative of the maximum amplification that can be achieved for a particular type of impulsive loading. Response Spectrum 2.5 2 1.5 Dimax II. 1 0.5 0 0 0.5 1 1.5 2 2.5 td/T i 819 3 3.5 4 4.5 Structural Engineering Analysis and Design Second Edition The above shows that the maximum dynamic amplification that can be produced from short duration impulse loadings is two! Maximum amplifications of higher modes are represented by points to the right of that for the fundamental mode. On inspection of the red curve representing the ramp up load in duration td, it is apparent that when the ramp is of a shorter duration td than the fundamental period T1 (i.e. td/T1 < 1.0), the amplification is large decreasing from 2.0 to 1.0 (no dynamic amplification) when the duration equals the period. Higher modes are less amplified as td/Ti becomes larger. If the duration is larger than the fundamental period (i.e. td/T1 > 1.0), the amplification will be small. The yellow curve with a large duration is simply a special case of the red curve with an instantaneous ramp (i.e. td/T1 = 0.0), hence causing a dynamic amplification of 2.0. In conclusion, if the ramp is such that it is gradual enough to be at least equal to the period of the fundamental mode (i.e. td/T1 > 1.0), the amplification can be minimized. On inspection of the green curve representing the impulsive loads, if the duration of the impulse td is close to the period of the fundamental mode T1, the amplification is large (~1.5). Higher modes are less amplified as td/Ti becomes larger. If the duration is much smaller than the fundamental period (td/T1 < ~0.4), the amplification is less than unity, and hence not even the static response is observed as the impulse to too fast for the structure to react. If the duration is much larger than the fundamental period (td/T1 > 2.0), the amplification is small. The yellow curve with a small duration is simply a special case of the green curve with an instantaneous impulse (i.e. td/T1 < ~0.2), hence causing a dynamic amplification of less than 1.0 (i.e. less than static response). In conclusion, if the impulsive load is much smaller in duration (td/T1 < ~0.4) or much larger in duration (td/T1 > 2.0) compared to the fundamental mode T1, the amplification can be minimized. The fact that impulsive loads cause little amplification can also be quantified more directly than employing the dynamic amplification. The response from a true impulse (t1/T < ~0.2) is readily obtained as the unit impulse function can be brought outside the Duhamel’s or Convolution Integral. The maximum modal response (not the dynamic amplification Di(t)) from an impulsive load (t1/T < 0.2), can be obtained simply as follows. ξ i (τ = t ) = h(t - τ) ξ i max = 1 M i ω ni ξ i max = 1 M i ω di ∫ τ= t τ= 0 ∫ τ= t τ= 0 ∫ τ= t τ= 0 p(τ)dτ φ i p(τ)dτ undamped φ i p(τ)dτ damped where φ i = mod al component at excitation point The above expression may seem to differ from the dynamic amplification approach where the denominator contains the modal stiffness, i.e. modal mass times the square of the natural circular frequency. This is because the above expression requires the explicit integration of the forcing function. The dynamic amplification approach differs in the sense that the integral (i.e. Duhamel’s Integral) is already classically integrated to obtain the expression D(t). Another equivalent interpretation of the above relationship is from the basic consideration of the conservation of momentum. The impacting particle (of small relative mass compared to mass of structure) imposes an impulse I onto the structure. The magnitude of I can be calculated as m∆v where m is the small mass and ∆v the change of velocity at impact. If there is no rebound ∆v is the approach velocity. Conservation of momentum at impact requires the initial velocity of the structural mass to be I/M. A lightly damped system then displays damped free vibration with an initial displacement of 820 Structural Engineering Analysis and Design Second Edition approximately I/(ωdM), or an initial velocity of approximately I/M or an initial acceleration of approximately Iωd/M. The general derivation of the impulse force is a science in itself. Simple considerations can however result in good approximations. As mentioned, an impacting particle (of small relative mass compared to mass of structure) imposes an impulse I = F∆t = m∆v onto the structure, where m and ∆v are known. Knowing that F∆t is the area under the impulse curve, making an estimate of the shape of the impulse curve and the duration ∆t, we can thus estimate the peak amplitude. Hence, the impulse curve is defined. Hence, if the structure is tuned such that the period of the fundamental mode is much less than the duration of the impulse (t1/T < 0.2), the amplification will be very low and can readily be ascertained using the above relationship. Of course, higher modes may be amplified more than the fundamental mode but would respond less because of the larger natural frequency ωni2. III. Higher modes are less significant then lower modes because of the higher natural frequency ωni2 in the expression for the modal response ξi. Hence, in order to reduce the total (starting transient and steady-state) response (by controlling the distribution of mass, stiffness and damping) to a ramped up loading or impulsive excitation, the following may be undertaken. I. The structural mass distribution, stiffness distribution and boundary conditions are modified to minimize the dynamic amplification factor of the fundamental mode, D1(t). Higher modes may have a greater dynamic amplification. But since ωni2 features in the denominator of the modal response expression ξi, the higher modes will produce a lower modal response (although the modal physical response could be significant). II. The mass distribution of the structure is increased in order to increase the modal masses (specifically of the modes with significant modal response ξi, but generally all), which in turn reduces the modal response ξi. This however will lower the natural frequencies and will affect the dynamic amplification factor, Di(t) of I. III. The stiffness distribution of the structure is increased in order to increase the natural frequencies ωni2 (specifically of the modes with significant modal response ξi, but generally all), which feature in the denominator of the modal response ξi expression. This will however affect the dynamic amplification factor, Di(t) of I. IV. The boundary conditions of the structure are altered in order to increase the natural frequencies ωni2 (specifically of the modes with significant modal response ξi, but generally all), which feature in the denominator of the modal response ξi expression. This will however affect the dynamic amplification factor, Di(t) of I. V. The location and direction of the applied load excitation is modified to not correspond to the large locations of the modes with significant modal response ξi in order to reduce the amplitude of the modal force, which in turn will reduce the modal response ξi. 821 Structural Engineering Analysis and Design Second Edition 5.6.1.3 Concepts of Forced Frequency Response of Deterministic Periodic Harmonic Base Excitations For a SDOF system subjected to base harmonic excitations u0sinωt, in absolute terms the response would be u 0 1 + (2ζω / ω n ) 2 u (t) = (1 − ω 2 ω 2n ) 2 + ( 2ζω / ω n ) 2 sin (ωt + β − θ ) θ = tan −1 2ζω / ω n (1 − ω 2 ω 2n ) Defining an expression for the relative transmissibility as the displacement response amplitude divided by the amplitude of the enforcing harmonic displacement u0, 1 + (2ζω / ω n ) Tr = 2 (1 − ω 2 ω 2n ) 2 + ( 2ζω / ω n ) 2 This is the displacement transmissibility expression. The acceleration transmissibility is exactly similar. A plot of Tr versus ω/ωn is somewhat similar to that of (magnitude of the) dynamic amplification D versus ω/ωn, except that all the curves of different ζ pass through the same point of Tr = 1.0 when ω/ωn = √2. Noting the curves after this point it is observed that damping tends to reduce the effectiveness of vibration isolation for frequency ratios greater than √2. Variation of Tr with Frequency Ratio For Different Damping Transmissibility, Tr 6 zhi=0 5 zhi=0.1 4 zhi=0.2 zhi=0.3 3 zhi=0.4 zhi=1.0 2 zhi=2.0 1 0 0 1 Frequency Ratio ω/ωn 2 822 Structural Engineering Analysis and Design Second Edition 5.6.1.4 Concepts of Forced Transient Response of Deterministic Base Excitations In a modal enforced motion transient response analysis, the modal response in modal coordinates ξi and the modal response in physical coordinates ui(t) are ξ i (t) = D i (t) & {φ }T [M ]{1}& p 0i u&0 u& = −D i (t) i 2 = D i (t )Γi 20 Ki ω ni M i ω ni where Γi = − {u i ( t )} = {φ i }ξ i ( t ) {φ i }T [M ]{1} Mi =− {φ i }T [M ]{1} {φ i }T [M ]{φ i } Thus whereby we had the following for the modal response in load excitations {φ } {p } p ξ i ( t ) = D i ( t ) 0i = D i ( t ) i 2 0 Ki ω ni M i T we now have the following for enforced base motion {φ } [M ]{1}& p 0i u&0 = −D i (t) i 2 Ki ω ni M i T ξ i (t) = D i (t) An exceptionally crucial observation is that whereby for load excitations the amplitude of the forcing vector {p0} may be sparse with only possibly one point with a value, that for enforced motion is quite different [M]{1} & u&0 with all components having a value. Thus, the enforced motion amplitude of modal force is special in the sense that the loading is uniformly distributed. Hence, higher modes will have lower amplitude of modal force because the positive and negative terms in the mode shape will cancel in the expression of the modal force. Thus, higher modes will have a lower overall contribution (but inter-storey response may be significant). This does not generally occur for load excitations, unless the loading is uniformly distributed. To reiterate, higher modes in load excitations may well be significant if the location of the excitation is such that it corresponds to the greater components of the eigenvector and hence making the modal force is prominent. On the contrary, higher modes in base excitations will not be significant (to the total base shear but may well be significant for inter-storey response) because of the distributed nature of the forcing vector, canceling positive and negative terms in the eigenvector and making the modal force not prominent. Because of the fact that the enforced based motion acceleration induces a force proportional to the mass and the base acceleration, clearly, higher masses would induce a greater force upon the structure. In enforced motion, the modal participation factor is defined and is analogous to the ratio of the load excitation amplitude of modal force p0i but bereft of or normalized by the amplitude of the loading vector p0 divided by the modal mass Mi. 823 Structural Engineering Analysis and Design Second Edition 5.6.1.5 Concepts of Forced Transient Response (Response Spectrum Analysis) of Random Non-Stationary Base Excitations The maximum modal response in modal space for mode i is computed as follows ξ i max ( t ) = Γi S D ξ& ( t ) = Γ S i max i V & ξ&i max ( t ) = Γi S A The maximum modal responses in physical space for mode i is then computed as follows {u imax (t)} = {φ i }ξ i max ( t ) = {φ i }Γi S D {u& (t)} = {φ }ξ& ( t ) = {φ }Γ S imax i i max i i V {& u&imax (t)} = {φ i }& ξ&i max ( t ) = {φ i }Γi S A An interesting point that could be made is the difference between the response spectrum method and the response due to enforced motion based on the dynamic amplification method. The maximum modal response from enforced base motion based on the dynamic amplification is ξ i max ( t ) = D i max (t )Γi & u&0 ω 2ni Comparing, hence the spectral displacement is S D = D i max (t ) & u&0 ω 2ni 824 Structural Engineering Analysis and Design Second Edition 5.6.2 Optimum Damping Distribution Damping can often be ignored for short duration loading such as crash impulses or shock blast because the structure reaches peak before significant energy has had time to dissipate. Damping is important for long duration loadings such as earthquakes, wind and loadings such as rotating machines, which continually add energy to the structure and is especially critical when the response at resonance is to be established, for it is only the damping which balances the externally applied force as the potential energy (stiffness) and the kinetic energy (mass) cancel each other. Two mathematical formulations of damping exist, namely (i) viscous damping c(du/dt), which is proportional to the response velocity (hence proportional to the forcing frequency), and (ii) structural damping iGku, which is proportional to the response displacement (hence independent of the forcing frequency) The choice of the damping formulation should depend on the actual real world damping mechanism that is to be modeled. However, it is often the case that the formulation adopted is dependent upon that which can be handled by the dynamic solution algorithm. Viscous damping can be incorporated in both time and frequency domain solutions schemes whilst structural damping can only be incorporated in frequency domain solution schemes. The structural and viscous damping can be incorporated at 3 different levels, namely elemental, modal and global levels. 5.6.2.1 Elemental Damping Mathematical Models Elemental damping damps all the structural modes of vibration accurately for all excitation frequencies irrespective of whether they are at resonance with the mode or not. Equivalent elemental damping introduces approximations. 5.6.2.1.1 Elemental Viscous Damping This damping formulation can be implemented in the time domain (SOL 109, SOL 112, SOL 129) or in the frequency domain (SOL 108, SOL 111) with CDAMP, CVISC, CBUSH or CBUSH1D elements. It will damp all the structural modes of vibration accurately (obviously some modes will be damped more than others) for all excitation frequencies irrespective of whether they are at resonance with the mode or not. The viscous damper is a device that opposes the relative velocity between its ends with a force that is proportional to velocity. The elemental viscous damping force is given by fd = c u& The user specifies the elemental damping constant c in Ns/m, which is constant in a CDAMP, CVISC, CBUSH or CBUSH1D element. A material is considered to be elastic when the stresses due to an excitation are unique functions of the associated deformation i.e. τ = Geγ. Similarly, a material is said to be viscous when the stress state depends only on the deformation rates i.e. τ = Gv γ&. Assuming no slip between the shear strain is related to the plunger motion by where td is the thickness of the viscous layer. Letting L and w represent the initial wetted length and width of the plunger respectively, the damping force is equal to 825 Structural Engineering Analysis and Design Second Edition Substituting for τ Finally, for fd = c u& The design parameters are the geometric measures w, L and td and the fluid viscosity, Gv. For analysis, it is necessary to (i) find the value of the damping parameters in practice to put into a computational model (ii) verify the damping parameters in the time or frequency domain computational model. These can be done by evaluating the response stress-strain curve of the element. The area under its response stress-strain curve represents the energy dissipated in an element. The displacement, velocity, acceleration and force are instantaneous quantities. Depicted for a SDOF system, if we know its velocity at any instant of time, the damping force at that instant is equal to the damping constant c multiplied by the velocity. Energy dissipated on the other hand is a cumulative quantity; hence the instantaneous force must be multiplied with an instantaneous differential displacement and summed over all the differential displacements. In the frequency domain, the energy dissipated by viscous damping during one cycle of harmonic vibration of forcing excitation p0sinωt is equal to the damping force multiplied the differential displacement, integrated over the single period of vibration. Hence, p0 / k Displacement response amplitude, D(ω)p 0 / k = (1 − ω2 ω2n ) 2 + ( 2ζω / ωn ) 2 Displacement response u p ( t ) = D(ω) p 0 / k sin (ωt − θ) Velocity response u&p ( t ) = D(ω)ωp 0 / k cos(ωt − θ) Force response = cu&p ( t ) Energy dissipated in one harmonic cycle of ω, E d = = ∫ t =0 ∫ cu&p ( t )du t =2π / ω t =0 ∫ =∫ = t =2π / ω t =2π / ω t =0 t =2π / ω t =0 cu&p ( t ) du dt dt cu&p ( t )dt 2 c(D(ω)ωp 0 / k cos(ωt − θ )) dt 2 t =2π / ω = c(D(ω)p 0 / k ) ω2 ∫ = c(D(ω)p 0 / k ) ω2 π ω 2 2 = πωc(D(ω)p 0 / k ) 2 826 t =0 cos 2 (ωt − θ )dt Structural Engineering Analysis and Design Second Edition The energy dissipated per cycle is directly proportional to the damping coefficient c, square of the response amplitude uˆ and proportional to the driving frequency ω. Ed = πωc uˆ 2 And the viscous damping coefficient is 1 ∆W 1 E d ζ= = 4π W 4π W Shock absorbers in vehicle suspensions are viscous dampers. Fluid is forced through orifices located in the piston head as the piston rod position is changed, creating a resisting force which depends on the velocity of the rod. The damping coefficient can be varied by adjusting the control valve. Radiation damping is a viscous damping mechanism occurring due to pressure wave radiation into medium surrounding the structure. This is a very efficient form of energy dissipation mechanism. If a plane wave is considered, then the energy transferred from the structure to the fluid per unit area per cycle is Ed = πωρc(D(ω)p0/k)2 Equating the energy dissipated per harmonic cycle for viscous damping and radiation damping, Ed viscous = πωc(D(ω)p0/k)2 = Ed radiation = πωρv(D(ω)p0/k)2 c = ρv For a radiation plane wave, the viscous damping c per unit surface area of the structure is ρv where ρ is the density and v the speed of sound in the medium into which the structure propagates the energy. Radiation into solid medium thus gives a high value for this damping and hence accounts for most of foundation damping in buildings. It is also an efficient mechanism for structures surrounded in liquid. For design, it is necessary to (i) find the range of the damping parameter for optimum damping of a particular mode For the design of explicit dampers, it is necessary to find the location and range of the damping parameter for optimum damping of a particular mode. The optimum location will clearly be at the position of the maximum components of the eigenvector. Optimum values of c depend on the optimum modal damping obtained for a particular range of damping constant. There is always a plateau where the values of the damping constant c will give the optimum (highest) modal damping. This plateau range is obtained computationally by running repetitive complex modal analysis (MSC.NASTRAN SOL 107) with varying damping constants, and observing the range which gives the optimum damping for the structural mode that is to be damped. 5.6.2.1.2 Elemental Structural Damping This damping formulation can be implemented ONLY in the frequency domain (SOL 108, SOL 111) on the MAT1 card or using CELAS or CBUSH elements. It will damp all the structural modes of vibration accurately (obviously some modes will be damped more than others) for all excitation frequencies irrespective of whether they are at resonance with the mode or not. The structural damping force is proportional to displacement and is in phase with velocity. The structural damping force is given by fd = iGEku In the frequency domain, the user specifies the damping loss factor GE and k in a MAT1, CELAS or CBUSH element. For analysis, it is necessary to (i) find the value of the damping parameters in practice to put into a computational model (ii) verify the damping parameters in the time or frequency domain computational model. These can be done by evaluating the response stress-strain curve of the element. The area under its response stress-strain curve represents the energy dissipated in an element. 827 Structural Engineering Analysis and Design Second Edition It can be shown that the energy dissipated in one harmonic cycle of ω by a structural damping element is Ed = πGEk uˆ 2 Structural damping is actually a general friction damping mechanism which allows for a variable magnitude of the friction force since it is proportional to the response displacement. This is contrasted with the less general friction damping mechanism i.e. Coulomb damping where the magnitude of the friction force is constant and limited. 5.6.2.1.3 Elemental Equivalent Viscous Damping for Structural Damping There no reason to implement this damping formulation in the frequency domain as elemental structural damping can be specified instead. It can be implemented in the time domain (SOL 109, SOL 112, SOL 129) on the MAT1 card or using CELAS or CBUSH elements, all with the specification of the ‘tie in’ frequency PARAM, W4. If PARAM, W4 is not specified, no equivalent viscous damping for structural damping will be implemented. This damping formulation will NOT damp any of the structural modes of vibration accurately except the solitary ‘tied in’ mode that will be damped accurately ONLY when the excitation frequency matches its natural frequency (i.e. at resonance). Hence, this damping formulation should NOT be used, a modal approach should be used for the time domain instead. Structural damping needs to be converted to equivalent viscous damping for solutions in the time domain by dividing the structural damping by the excitation frequency. 1 f d = G E ku& ω Although this equivalence can be implemented exactly in the frequency domain with the frequency dependent damping capability of the CBUSH element, this is unnecessary as structural damping can be defined in the frequency domain anyway. In the time domain, this requires the definition of a ‘tie in’ forcing frequency, chosen to correspond to a structural mode that is most prominent for the response (i.e. that which shows the greatest modal response with respect to time, a characteristic that can be obtained using SDISP, SVELO or SACCE in the modal solution), i.e. ω = ω1. Hence, in the time domain, the user specifies the GE, k and ω1 from which c = GEk /ω1 in a MAT1, CELAS or CBUSH element, all with PARAM, W4. 1 fd = G E ku& ω1 For analysis, it is necessary to (i) find the value of the damping parameters in practice to put into a computational model (ii) verify the damping parameters in the time or frequency domain computational model. These can be done by evaluating the response stress-strain curve of the element. The area under its response stress-strain curve represents the energy dissipated in an element. The equivalence is obtained by equating the energy dissipated per harmonic cycle for viscous damping and structural damping as follows. Ed viscous = πωc(D(ω)p0/k)2 = Ed structural = πGEk(D(ω)p0/k)2 ceq = GEk / ω 828 Structural Engineering Analysis and Design Second Edition 5.6.2.1.4 Elemental Equivalent Viscous Damping for Velocity-Squared Damping This damping formulation can be implemented approximately in the frequency domain (SOL 108, SOL 111) with CBUSH elements. It can be implemented approximately in the time domain (SOL 109, SOL 112) with CDAMP, CVISC, CBUSH or CBUSH1D elements. It should not be used in a nonlinear time domain solution (SOL 129) as the nonlinear (velocity squared) viscous damping can be modeled exactly in the nonlinear solution scheme with CBUSH1D elements. Velocity-squared damping is directly proportional to the square of the velocity and opposes the direction of motion. f d = au&2 In a nonlinear time domain solution SOL 129, the user specifies ‘a’ in CBUSH1D. In the frequency domain SOL 108 and SOL 111, the user specifies ‘a’, variable ω and a constant displacement response amplitude uˆ from which ceq = (8/3π)a uˆ ω in an excitation frequency dependent CBUSH. 8 fd = auˆωu& 3π In the linear time domain SOL 109 and SOL 112, the user specifies ‘a’, a constant displacement response amplitude uˆ and a constant forcing frequency ω, the latter of which is chosen to correspond to a structural mode that is most prominent for the response (i.e. that which shows the greatest modal response with respect to time, a characteristic that can be obtained using SDISP, SVELO or SACCE in the modal solution), i.e. ω = ω1 from ceq = (8/3π)a uˆ ω1 in a CDAMP, CVISC, CBUSH or CBUSH1D element. 8 fd = auˆω1 u& 3π For analysis, it is necessary to (i) find the value of the damping parameters in practice to put into a computational model (ii) verify the damping parameters in the time or frequency domain computational model. These can be done by evaluating the response stress-strain curve of the element. The area under its response stress-strain curve represents the energy dissipated in an element. The equivalence is obtained by equating the energy dissipated per harmonic cycle for viscous damping and velocity-squared damping as follows. For a linear viscous damper, the steady-state energy dissipated during one harmonic cycle is Ed = πcω uˆ ² where uˆ is the amplitude of steady-state displacement, and ω is the excitation frequency i.e. the steady state response frequency. For a linearized velocity squared damper, steady-state energy dissipated during harmonic cycle Ed = (8/3)aω² uˆ ³ where a is the velocity-squared damping constant (Ns2/m2), and uˆ is the amplitude of the steady-state displacement response. By equating the dissipated energies, the equivalent viscous damping coefficient for the velocity-squared damper is ceq = (8/3π)a uˆ ω. Industrial hydraulic dampers are velocity-squared dampers. Velocity squared damping models the behavior observed when systems vibrate in fluid or when a fluid is rapidly forced through an orifice. For design, it is necessary to (i) find the range of the damping parameter for optimum damping of a particular mode For the design of explicit dampers, it is necessary to find the location and range of the damping parameter for optimum damping of a particular mode. The optimum location will clearly be at the position of the maximum components of the eigenvector. Optimum damping constant ‘a’ can be obtained from repetitive SOL 129 analyses. Alternatively, assuming uˆ and choosing ω = ω1 so that ceq = (8/3π)a uˆ ω1, repetitive SOL 107 can be run for numerous ‘a’ values and hence ceq, until the optimum damping plateau is obtained. 829 Structural Engineering Analysis and Design Second Edition 5.6.2.1.5 Elemental Equivalent Viscous Damping for Coulomb Damping This damping formulation can be implemented approximately in the frequency domain (SOL 108, SOL 111) with CBUSH elements. It can be implemented approximately in the time domain (SOL 109, SOL 112) with CDAMP, CVISC, CBUSH or CBUSH1D elements. It should not be used in a nonlinear time domain solution (SOL 129) as the damping can be modeled exactly in the nonlinear solution scheme with the CGAP (contact and) friction element. It is assumed that the (constant and limited) force resisting the direction of motion is proportional to the normal force FN between the sliding surfaces, independent of the magnitude of velocity but is in phase with the velocity (hence the sign of velocity term). where F is the limiting Coulomb force magnitude and is equal to µFN where FN is the normal contact force and µ the coefficient of friction. In a nonlinear time domain solution SOL 129, the user specifies the coefficient of friction, µ in a CGAP contact-friction element. In the frequency domain SOL 108 and SOL 111, the user specifies µ, FN, variable ω and variable uˆ from which c is calculated from ceq = 4µFN/(πω uˆ ). Due to the nature of the Coulomb force being in phase with the velocity, an equivalent viscous damping model can easily be used in a CBUSH element. 4µFN fd = u& πωuˆ where FN is the normal force, µ the coefficient of friction and uˆ the harmonic response amplitude. In the linear time domain SOL 109 and SOL 112, a constant displacement response uˆ and forcing frequency ω is required, the latter of which is chosen to correspond to a structural mode that is most prominent for the response (i.e. that which shows the greatest modal response with respect to time, a characteristic that can be obtained using SDISP, SVELO or SACCE in the modal solution), i.e. ω = ω1. In the time domain, the user specifies µ, FN, ω1 and uˆ from which ceq = 4µFN/(πω1 uˆ ) in a CDAMP, CVISC, CBUSH or CBUSH1D element. 4µFN fd = u& πωuˆ For analysis, it is necessary to (i) find the value of the damping parameters in practice to put into a computational model (ii) verify the damping parameters in the time or frequency domain computational model. These can be done by evaluating the response stress-strain curve of the element. The area under its response stress-strain curve represents the energy dissipated in an element. The energy dissipated is proportional to the friction force and the amplitude of vibration as follows. Ed = 4µFN uˆ Coulomb damping or dry friction damping is found wherever sliding friction is found in machinery, laminated springs or bearings. Coulomb damping is also used to model joint damping mechanisms. Joint damping is found in highly assembled structures. 830 Structural Engineering Analysis and Design Second Edition 5.6.2.1.6 Elemental Equivalent Structural Damping for Hysteretic Damping This damping formulation can be implemented ONLY in the frequency domain (SOL 108, SOL 111) on the MAT1 card or using CELAS or CBUSH elements. It will damp all the structural modes of vibration accurately (obviously some modes will be damped more than others) for all excitation frequencies irrespective of whether they are at resonance with the mode or not. It should not be used in a nonlinear time domain solution (SOL 129) as the damping can be modeled exactly in the nonlinear solution scheme with an elastic-plastic hysteretic material model MATS1 (TYPE PLASTIC). The form of the damping force-deformation relationship depends on the stress-strain relationship for the material and the make-up of the device. For an elastic-perfectly plastic material, the limiting values are Fy, the yield force, and uy, the displacement at which the material starts to yield; kh is the elastic damper stiffness. The ratio of the maximum displacement to the yield displacement is referred to as the ductility ratio and is denoted by µ. In a nonlinear time domain solution SOL 129, the user specifies the initial stiffness kh, the yield force Fy and the ductility ratio µ or the ultimate strain in a MATS1 (TYPE PLASTIC). In the frequency domain SOL 108 and SOL 111, the user specifies the equivalent structural damping loss factor GE for the hysteretic damper as GE = 2(µ−1) where µ is the ductility ratio in a MAT1, CELAS or CBUSH element. For analysis, it is necessary to (i) find the value of the damping parameters in practice to put into a computational model (ii) verify the damping parameters in the time or frequency domain computational model. These can be done by evaluating the response stress-strain curve of the element. The area under its response stress-strain curve represents the energy dissipated in an element. The work per cycle for hysteretic damping is Hysteretic damping is due to the inelastic deformation of the material composing the device. Hysteretic damping is also offered by hysteretic damper brace elements. For design, it is necessary to (i) find the range of the damping parameter for optimum damping of a particular mode For the design of explicit hysteretic damper brace elements, it is necessary to find the location and range of the damping parameter for optimum damping of a particular mode. The optimum location will clearly be at the position of the maximum components of the eigenvector. Optimum ductility ratio µ can be obtained from repetitive SOL 129 analyses. Alternatively, assuming repetitive SOL 107 can be run for numerous GE values and hence µ, until the optimum damping plateau is obtained. 831 Structural Engineering Analysis and Design Second Edition 5.6.2.1.7 Elemental Equivalent Structural Damping for Viscoelastic Damping This damping formulation can be implemented ONLY in the frequency domain (SOL 108, SOL 111) on the CBUSH elements or in SOL 108 with MAT1 and TABLEDi (with the SDAMPING Case Control Card). It should not be used in a nonlinear time domain solution (SOL 129) as the damping can be modeled exactly in the nonlinear solution scheme with the CREEP material model. Viscoelastic materials are characterized by the shear modulus G (which relates to a stiffness k) and the loss factor, GE both of which are temperature, strain and frequency dependent. The ratio is the shear loss tangent. A material is considered to be elastic when the stresses due to an excitation are unique functions of the associated deformation i.e. τ = Geγ. Similarly, a material is said to be viscous when the stress state depends only on the deformation rates i.e. τ = Gv γ&. An elastic material responds in phase with excitation whilst a viscous element responds 90 degrees out of phase. Hence a viscoelastic element responds 0 – 90 degrees out of phase with the excitation. In the frequency domain SOL 108 and SOL 111, the user specifies the excitation frequency dependent stiffness, k(ω) and the excitation frequency dependent loss factor, GE(ω) in a CBUSH element. Alternatively in SOL 108, SDAMPING = n to reference TABLEDi Bulk Data entry MAT1 with G = GREF (reference modulus) and GE = gREF (reference element damping) A TABLEDi Bulk Data entry with an ID = n is used to define the function TR(f) A TABLEDi Bulk Data entry with an ID = n+1 is used to define the function TI(f) where the stiffness matrix of the viscoelastic elements For analysis, it is necessary to (i) find the value of the damping parameters in practice to put into a computational model (ii) verify the damping parameters in the time or frequency domain computational model. These can be done by evaluating the response stress-strain curve of the element. The area under its response stress-strain curve represents the energy dissipated in an element. 832 Structural Engineering Analysis and Design Second Edition Viscoelastic damping is present in most materials, albeit at very small levels. This is of course present in both the elastic and plastic range of the material deformation and their values are presented below. Material Steel Cast iron Aluminium Lead Rubber Glass Concrete Loss Factor, GE 0.001 – 0.008 0.003 – 0.03 0.00002 – 0.002 0.008 – 0.014 0.1 – 0.3 0.0006 – 0.002 0.01 – 0.06 Viscoelastic damping is utilized in constrained layer damping for structural and aeronautical applications. Examples include SUMITOMO-3M, SWEDAC and bituthene. This method works best when the constrained layer is put into shear and therefore the most effective location of such a layer is at the neutral axis of the floor beam or slab where the complementary shear stresses are high. Typical visco-elastic materials are fairly flexible and can exhibit significant creep. Therefore introduction of a constrained layer means that the structure is more flexible than it would be if it were monolithic. For static loads therefore these types of layers are not ideal, and so a compromise must often be reached. Constrained layer damping has quite often been applied to excessively lively existing structures by adding an extra “cover plate” on top of or beneath the existing floor in order to constrain a layer of visco-elastic material. Slab Truss end The stiffness k of a (zero-length two orthogonal horizontal direction) spring representing an area A of viscoelastic constrained layer material is AG/t where t is the thickness and G the shear modulus. The variation of G and the loss factor GE with temperature, excitation frequency has been established for bituthene. Temperature has dramatic effect on G but little on GE. The material properties to use based on interpolation of test results at 20 °C and a frequency of 5Hz are thus Shear Modulus G = 1.17 MPa Loss factor GE = 0.75 (at very small strains) For design, it is necessary to (i) find the range of the damping parameter for optimum damping of a particular mode Optimum damping parameters k and GE can be obtained from repetitive SOL 107 analyses, until the optimum damping plateau is obtained. For constrained layer viscoelastic damping, repetitive SOL 107 can be run until the value of k (and hence the thickness t since k = AG/t) that yields the optimum damping is obtained. 833 Structural Engineering Analysis and Design Second Edition 5.6.2.2 Modal Damping Mathematical Models Modal damping damps all the structural modes of vibration specified with a modal damping accurately at all excitation frequencies irrespective of whether they are at resonance with the mode or not. Equivalent modal damping damps the structural modes of vibration specified with a modal damping accurately ONLY when the excitation frequency matches the frequency of each particular natural mode. Note that the modal damping approach will not be valid if the modes are significantly complex, i.e. different parts of the structure are out-of-phase (reaching their maximum at different instances) in a particular mode as the modal damping values are applied on the real modes. Damping elements with high values of damping can result in the structure having totally different damped modes of vibration. For instance, a cable with a damper element with a very high damping coefficient attached to its center will behave as two separate cables, the damper element effectively producing a fixity at the center of the cable. This changes the fundamental mode shape of the cable from one of a low frequency to two cable mode shapes of higher fundamental frequency. For analysis, it is necessary to (i) find the value of the damping parameters in practice to put into a computational model (ii) obtain modal damping values from a set of explicit element dampers There are various methods of obtaining the modal damping coefficients in practice and from finite element models damped with individual explicit viscous or structural damping elements. Complex modal analysis (SOL 107) can be performed to ascertain the structural modal damping coefficients Gi for each and every mode. Alternatively, a forced frequency response analysis (SOL 108 or SOL 111) can be performed with a harmonic loading from which the modal damping coefficient can be ascertained in a variety of methods from the FRF. The methods of obtaining the damping from the FRF are: (i) the half-power bandwidth method which approximates the modal damping in lightly-damped structures (ζ < 0.1) where the ith modal damping coefficient is ζi = (ii) f i 2 − f i1 2f i where fi1 and fi2 are the beginning and ending frequencies of the half-power bandwidth defined by the maximum response divided by √2. The half-power bandwidth method assumes a SDOF response. the (magnitude of the) dynamic amplification factor at resonance method 1 = Dynamic Amplification Factor At Resonance of ith mode, D i resonant 2ζ i = Maximum Displacement Response Amplitude of ith mode, D i resonant p 0 /k Static Displacement Response Amplitude, p 0 /k Another method of obtaining modal damping estimates is the logarithmic decrement method. In order to obtain the values of ζi, a transient analysis (SOL 109, SOL 112, SOL 129) can be performed and successive peaks can be observed from the free vibration response. The free vibrational analysis can be set up using an initial displacement condition or an impulsive force that ramp up and down quickly with respect to the dominant period of the response and/or other natural frequencies of interest. The logarithmic decrement, δ is the natural log of the ratio of amplitude of two successive cycles of free vibration. Then the damping ratio is ζ≈ δ 2π The logarithmic decrement method assumes a SDOF response. Modal damping of higher modes requires signal filtering of the response time history. 834 Structural Engineering Analysis and Design Second Edition 5.6.2.2.1 Modal Viscous Damping This damping formulation can be implemented in the modal time domain (SOL 112) with the SDAMPING Case Control Command and the TABDMP1 entry. It can also be implemented in the modal frequency domain (SOL 111) with SDAMPING Case Control Command, the PARAM, KDAMP and the TABDMP1 entry. It will damp all the structural modes of vibration specified with a modal damping value accurately for all excitation frequencies irrespective of whether they are at resonance with the mode or not. The damping force is given by f id = ζ i ( 2M i ω n i ) (iωξ i (ω)) The user specifies ζi. 5.6.2.2.2 Modal Structural Damping This damping formulation cannot be implemented in the modal time domain (SOL 112). It can be implemented in the modal frequency domain (SOL 111) with the SDAMPING Case Control Command, the PARAM, KDAMP and the TABDMP1 entry where it will damp all the structural modes of vibration specified with a modal damping value accurately for all excitation frequencies irrespective of whether they are at resonance with the mode or not. The damping force is given by f id = iG i K i ξ i (ω) The user specifies Gi. 5.6.2.2.3 Modal Equivalent Viscous Damping for Modal Structural Damping There no reason to implement this damping formulation in the modal frequency domain as modal structural damping can be specified instead. It can be implemented in the modal time domain (SOL 112) with the SDAMPING Case Control Command and the TABDMP1 entry. This damping formulation will damp all modes specified with a modal damping value accurately ONLY when the excitation frequency matches the natural frequency of the particular mode (i.e. at resonance), often an acceptable approximation. This modal damping formulation is extremely useful in modelling structural damping in time domain solutions. Time domain solutions, be they direct or modal cannot handle structural damping. Incorporating elemental structural damping within a time domain solution requires a ‘tie in’ frequency, hence damping the different modes inaccurately. The best method would be to use a modal approach, i.e. SOL 112 where modal damping can be specified and internally automatically converted into modal viscous damping. All the modes are then damped accurately when the excitation frequency matches the natural frequency of the particular mode. Again, the method works if the modes are only slightly complex, as the modal damping estimates are applied onto the real modes. The following presents the appropriate conversion between modal viscous and modal structural damping. It will be shown that the two forms of damping are only theoretically equivalent when the forcing frequency ω equals the natural frequency of the structural mode of vibration ωn. This is proven mathematically and pictorially below showing the variation of viscous and structural damping with forcing frequency. 835 Structural Engineering Analysis and Design Second Edition fd Viscous damping Structural damping Forcing frequency, ω ω = ωn For the viscous damping force to equal the structural damping force f viscous = f structural cu&= iGku icωu = iGku The damping constant c is specified as a percentage of critical damping ζ of a particular structural mode iω(ζ2mωn)u = iGku ω(ζ2mωn) = Gk If and only if ω = ωn ωn(ζ2mωn) = Gk ζ2mωn2 = Gk ζ2mk / m = Gk ζ=G/2 Although the two damping formulations are only identical the resonances ω = ωn and not for other forcing frequencies, damping is most critical at resonance when ω ≈ ωn (when the inertial and stiffness forces cancel) and so the switch between viscous and structural formulations is often acceptable in practice. Whenever possible, the damping formulation chosen (i.e. whether viscous or structural) should be such as to simulate the actual real-world damping mechanism. Nevertheless, the use of viscous damping to simulate structural damping (and vice versa for that matter) is possible, but it must be borne in mind that the conversion is only accurate at resonance when the structural modal frequencies equal the forcing frequencies. From above, it is obvious that the use of a viscous damping formulation to represent a structural damping mechanism will overestimate damping when the forcing frequency ω is higher than ωni and underestimate damping when the forcing frequency ω is lower than ωni. Conversely, the use of a structural damping formulation to represent a viscous damping mechanism will underestimate damping when the forcing frequency ω is higher than ωni and overestimate damping when the forcing frequency ω is lower than ωni. 836 Structural Engineering Analysis and Design Second Edition 5.6.2.3 Global Damping Mathematical Models Global damping formulations are the crudest method of modelling damping. This method does not damp all the natural modes accurately because it is often based on the damping estimates of either one or two modes only. These modal estimates are obtained using methods of obtaining modal damping values described previously. 5.6.2.3.1 Global Viscous Damping (Mass Proportional Damping) The global (mass proportional) viscous damping force is given by [F]d = [C]{u&} = α[ M ]{u&} = ζ i 2ω ni [M ]{u&} The user specifies α. The values of ζi and ωni are based one mode only, usually the first fundamental mode which usually dominates the response. Hence, the method tends to underestimate damping in modes of higher than ωni frequencies and overestimate damping in modes of lower than ωni frequencies. Fd Viscous damping Fd Underestimated Overestimated Modal frequency, ωni ωni 5.6.2.3.2 Global Structural Damping This damping formulation can ONLY be implemented in the frequency domain (SOL 108, SOL 111) using PARAM, G. It will damp all the structural modes of vibration accurately (obviously some modes will be damped more than others) for all excitation frequencies irrespective of whether they are at resonance with the mode or not if and only if all the deformable elements have associated structural damping of the same value. The global structural damping force is given by [F]d = iG[K ]{u} The user specifies G. 5.6.2.3.3 Global Equivalent Viscous Damping for Structural Damping (Stiffness Proportional Damping) There no reason to implement this damping formulation in the frequency domain as elemental structural damping and/or modal structural damping can be specified instead. It can be implemented in the time domain (SOL 109, SOL 112, SOL 129) using PARAM, G with the specification of the ‘tie in’ frequency PARAM, W3. If PARAM, W3 is not specified, no equivalent viscous damping for structural damping will be implemented. This damping formulation will NOT damp any of the structural modes of vibration accurately 837 Structural Engineering Analysis and Design Second Edition except the solitary ‘tied in’ mode that will be damped accurately ONLY when the excitation frequency matches its natural frequency (i.e. at resonance). Hence, this damping formulation should NOT be used, a modal approach should be used for the time domain instead. The global (stiffness proportional) viscous damping force is given by [F]d = β[K ]{u&} = 2ζ i [K ]{u&} ω ni The user specifies β. The values of ζi and ωni are based one mode only, usually the first fundamental mode which usually dominates the response. Hence, the method tends to overestimate damping in modes of higher than ωni frequencies and underestimate damping in modes of lower than ωni frequencies. Fd Underestimated Overestimated Viscous damping Fd Modal frequency, ωni ωni This method is crudely used to model the structural damping mechanism in a global viscous formulation. This is so because, from the above equation [F]d = β[K ]{u&} = 2ζ i [K ]{u}iω ω ni When ω = ω ni [F]d = i2ζ i [K ]{u} = iG i [ K ]{u} As mentioned, a viscous formulation to model structural damping will overestimate damping when the forcing frequency ω is higher than ωni and underestimate damping when the forcing frequency ω is lower than ωni. This is even more exaggerated here as the damping estimate is based upon just one mode. 5.6.2.3.4 Global Equivalent Viscous Damping for Viscous and Structural Damping (Mass and Stiffness Proportional Rayleigh Damping) The Rayleigh proportional viscous damping force is given by [F]d = [α[M] + β[K]]{u&} The user specifies α and β. 838 Structural Engineering Analysis and Design Second Edition The factors α and β are chosen to give the correct damping at two excitation frequencies. For a specified damping factor ζ at an excitation frequency ω then ζ= 1α   + βω  2ω  And using this at 2 frequencies ωr and ωs with the required damping factors ζr and ζs respectively gives α = 2ω r ω s β=2 ζ s ω r − ζ r ωs ω 2r − ω s2 ζ r ω r − ζ s ωs ω 2r − ω s2 The method is based on the damping coefficients ζr and ζs of two distinct modes ωr and ωs. By specifying ζr = ζs, all structural natural modes between modal frequencies ωr and ωs will have damping less than at modes ωr and ωs. Fd Viscous damping Fd ωr 5.6.2.4 ωs Modal frequency, ωn Damping Formulation Conclusions The choice of using a viscous damping formulation or a structural damping formulation should depend on the actual real world damping mechanism being modeled. Elemental damping formulations damp all modes accurately at all excitation frequencies. If an equivalent elemental damping formulation is used, then not all natural modes will be damped accurately. Modal damping formulations damp all modes specified with a modal damping accurately at all excitation frequencies. Equivalent modal damping formulations damp all modes specified only when the excitation frequency matches the natural frequency of the mode. The use of a modal viscous damping formulation to represent a modal structural damping mechanism will overestimate the modal damping when the forcing frequency ω is higher than ωni and underestimate the modal damping when the forcing frequency ω is lower than ωni. Conversely, the use of a modal structural damping formulation to represent a modal viscous damping mechanism will underestimate the modal damping when the forcing frequency ω is higher than ωni and overestimate the modal damping when the forcing frequency ω is lower than ωni. Global proportional damping will damp only one or two structural modes accurately. Global mass proportional viscous damping tends to underestimate damping in modes of higher than ωni frequencies and overestimate damping in modes of lower than ωni frequencies. Global structural damping will damp all modes accurately at all excitation frequencies if all the deformable elements exhibit structural damping of the same value. Global stiffness proportional viscous damping tends to overestimate damping in modes of higher than ωni frequencies and underestimate damping in modes of lower than ωni frequencies. Global Rayleigh damping can be made, by specifying ζr = ζs, to damp all modes between modal frequencies ωr and ωs to have damping less than at modes ωr and ωs. 839 Structural Engineering Analysis and Design Second Edition 5.6.3 GL, ML Base Isolation Systems Base isolation systems are used to minimize the effect of seismic support motion on structures and nonstructural elements and to reduce machine induced loadings on foundations. 5.6.3.1 Controlling Displacement Response From Harmonic Load Excitations We reiterate that the dynamic amplification factor D(ω) for applied harmonic loading p0sinωt on a SDOF system is Dynamic Amplification Factor, D Variation of D with Frequency Ratio For Diffe rent Damping 6 5 4 zhi=0 zhi=0.1 D i (ω) = zhi=0.2 3 2 1 0 zhi=1 zhi=2 0 1 D i max = (1 − ω ( 1 2 / ω ni 1 2ζ 1 − ζ 2 ) 2 2 + (2ζ i ω / ω ni ) ; 2 ) 2 Frequency Ratio ω / ω n The corresponding maximum displacement response of the SDOF system is umax = Dimax(p0/k). Dimax occurs when ω/ωn = (1-2ζ2)1/2. Clearly, if ωn is flexible (i.e. low) enough such that D(ω) is less than unity (the exact location varies with the amount of damping, being at ω/ωn = 1.4 for ζ = 0.0), the steady-state dynamic response will be less than the static response and the externally applied harmonic dynamic load excitation is well controlled for the displacement response. 5.6.3.2 Controlling Acceleration Response From Harmonic Load Excitations Now, it may also be desirable to limit the maximum acceleration amplitude. The acceleration response is simply the second derivative (with respect to time) of the displacement response. Hence the maximum acceleration response will be amax = ω2Dimax(p0/k) = (ω/ωn)2Dimax(p0/m). ω /ω ω n)^2.D(ω ω ) with Variation of (ω Frequency Ratio For Different Damping 7 (ω /ω n)^2.D(ω ) 6 zhi=0 zhi=0.1 zhi=0.2 zhi=1 zhi=2 5 4 3 2 1 0 0 1 2 3 Frequency Ratio ω /ω n 840 (ω / ω ni )2 D i (ω) = (ω / ω ni )2 D i max = (1 − ω ( (ω / ω ni )2 2 / ω ni 1 2ζ 1 − ζ 2 ) ) 2 2 + (2ζ i ω / ω ni ) ; 2 Structural Engineering Analysis and Design Second Edition Note that the behaviour of (ω/ωn)2Di(ω) for small and large ω/ωn is opposite to that of Di(ω). The maximum is the same but the location is different. The ratio p0/m is the acceleration of the mass if the mass is unrestrained. Hence (ω/ωn)2Di(ω) approaches unity for large (ω/ωn)2. The term (ω/ωn)2Di(ω) is then the multiplier to p0/k accounting for the time varying nature of the loading and the stiffness and damping of the system. Clearly, ω/ωn needs to be such that (ω/ωn)2Di(ω)p0/m is within the acceptable acceleration limit. 5.6.3.3 Base Isolation - Controlling Displacement Response From Harmonic Base Enforced Motion As described in Section 4.5.4.4, for a SDOF system subjected to base harmonic excitations u0sinωt, in absolute terms the response would be u 0 1 + (2ζω / ω n ) u (t) = (1 − ω 2 ω 2n ) 2 2 + ( 2ζω / ω n ) 2 sin (ωt + β − θ ) θ = tan −1 2ζω / ω n (1 − ω 2 ω 2n ) β = tan −1 ( 2ζω / ω n ) Defining an expression for the displacement transmissibility as the absolute displacement response amplitude divided by the amplitude of the enforcing harmonic displacement u0, Tr = 1 + (2ζω / ω n ) 2 (1 − ω 2 ω 2n ) 2 + ( 2ζω / ω n ) 2 This is the (absolute) displacement transmissibility expression. When we design for the displacement response, it is usually the relative response that we are concerned with. Now the steady state solution for the relative (to base) displacement is u 0 ω 2 / ω 2n u r (t ) = (1 − ω 2 ω 2n ) + ( 2ζω / ω n ) 2 2 sin (ωt − θ ) θ = tan −1 2ζω / ω n (1 − ω 2 ω 2n ) This expression is numerically equivalent to (ω/ωn)2Di(ω) and is shown below. ω /ω ω n)^2.D(ω ω ) with Variation of (ω Frequency Ratio For Different Damping 7 (ω /ω n)^2.D(ω ) 6 zhi=0 zhi=0.1 zhi=0.2 zhi=1 zhi=2 5 4 3 2 1 0 0 1 2 3 Frequency Ratio ω /ω n Clearly for design, ω/ωn needs to be such that (ω/ωn)2Di(ω)u0 is within the acceptable relative displacement limit. Note that for large ω/ωn values the expression approaches unity and hence the relative displacement response approaches the displacement of the base motion and needs to be designed for. 841 Structural Engineering Analysis and Design Second Edition 5.6.3.4 Base Isolation - Controlling Acceleration Response From Harmonic Base Enforced Motion The acceleration transmissibility (absolute acceleration response amplitude divided by the amplitude of the enforcing harmonic acceleration) is exactly similar to the (absolute) displacement transmissibility. 1 + (2ζω / ω n ) Tr = 2 (1 − ω 2 ω 2n ) 2 + ( 2ζω / ω n ) 2 This formula is effective to determine the natural frequency (hence stiffness) and damping of an isolation system knowing the input displacement or acceleration and the maximum acceptable dynamic acceleration that the structural component can be subjected to. Remember that only when damping is small that the maximum transmissibility can be approximated to occur at resonance. When damping is high, it is imperative that the transmissibility expression be differentiated or plotted (also use cannot be made of ω = ωn(1-2ζ2)1/2 as this is based on differentiating and maximizing the (magnitude of the) dynamic amplification factor, D(ω)). A plot of Tr versus ω/ωn is somewhat similar to that of (magnitude of the) dynamic amplification D versus ω/ωn, except that all the curves of different ζ pass through the same point of Tr = 1.0 when ω/ωn = √2. Noting the curves after this point it is observed that damping tends to reduce the effectiveness of vibration isolation for frequency ratios greater than √2. Variation of Tr with Frequency Ratio For Different Damping Transmissibility, Tr 6 zhi=0 5 zhi=0.1 4 zhi=0.2 zhi=0.3 3 zhi=0.4 zhi=1.0 2 zhi=2.0 1 0 0 1 Frequency Ratio ω/ωn 2 On investigating the transmissibility expression, we can design the supporting system for vibration isolation. The transmissibility is unity when the supporting system is infinitely stiff with respect to the loading frequency. The transmissibility is also unity when the frequency ratio is √2. If the supporting system is designed such that the frequency ratio is less than √2 but greater than 0, the transmissibility is greater than one, which means that the supporting system actually makes matters worse as far as vibration isolation is concerned. When the frequency ratio is greater than √2, it is seen that the transmissibility is smaller than unity and hence, the supporting system functions as a vibration isolator. Damping is seen to be advantages only in the region when the frequency ratio is less than √2 (where a spring mounting supporting system makes matters worse) and not when the frequency ratio is greater than √2 (where a spring mounting supporting system acts as a effective vibration isolator). This is not so important actually as the undesirable effects of high values of damping at frequency ratios greater than √2 is not so great especially at even higher frequency ratios, i.e. achieved by making the supporting system even more flexible. 842 Structural Engineering Analysis and Design Second Edition Also, in the unfortunate circumstance that the resonance region of frequency ratio less than √2 is somehow attained; high levels of damping are extremely effective. For good isolation, it is often recommended to design the supporting system for a frequency ratio of at least 3. An example of isolation systems in practice occurs in the case of the EUROSTAR train. Bogie 1 Typical Bogie Bogie 9 40.021 27.000 32.102 Ks kN/m 870 580 1250 Cs kNs/m 20 2 20 Mb tonne 3.025 3.250 3.200 Ib 2.800 2.800 2.800 Kp kN/m 2200 2075 1560 Cp kNs/m 12 12 12 a 3.0 3.0 3.0 2.128 2.095 2.113 M tonne tm² m Mw tonne The primary (bogie) suspension system has a natural frequency of about 5.7Hz, hence filtering frequencies higher than √2 x 5.7 = 8.1Hz. The secondary (deck) suspension system has a natural frequency of about 0.7Hz, hence filtering frequencies higher than √2 x 0.7 = 1.0Hz. 843 Structural Engineering Analysis and Design Second Edition Below is the modulus FFT of the acceleration response showing clearly the dominant frequency components of the response at the wheels, bogie and train deck. Another reason to employ isolation is to isolate rail-induced vibrations through the ground onto submerged structures or adjacent structures. The frequency content ranges from 1Hz to 150-200Hz. Structural vibrations occur due the 8Hz to 20Hz frequencies. Railway excitations have a pronounced frequency band between 40Hz and 80Hz, causing significant acoustic phenomena (structure borne sound). Note that noise can be detected above a frequency of about 16Hz. Vibration isolation devices typically ranging from 8Hz to 12Hz can be used to isolate frequencies above these. Road traffic also induces vibration with a frequency range from 1 to 200-400Hz but does not, in contrast with railinduced vibrations, exhibit pronounced frequency components. 5.6.3.5 Base Isolation – Controlling Force Transmitted Into Foundation From Harmonic Load Excitations The force transmissibility (force response amplitude divided by the amplitude of the enforcing harmonic force of p0sinωt, i.e. p0) is also exactly similar to the (absolute) displacement transmissibility. Tr = 1 + (2ζω / ω n ) 2 (1 − ω 2 ω 2n ) 2 + ( 2ζω / ω n ) 2 The transmissibility expression can be used for the force induced by a rotating machine into the supporting structure. Design supporting system such that ω/ωn = √2 for no dynamic effects. Note that the transmissibility expression is only valid for the force transmitted if the foundation is rigid. If the foundation is not rigid, then the supporting system must be even more flexible in order to provide the same level of protection as when the foundation is rigid. 844 Structural Engineering Analysis and Design Second Edition 5.6.4 GL, ML Tuned Mass Damper (TMD) Systems The TMD is a device consisting of a mass, spring and damper to reduce mechanical vibrations. The frequency and damping of the TMD is tuned so that when the structure resonates at a particular frequency, the TMD vibrates outof-phase transferring the energy from the primary system (i.e. the structure) to the secondary system (i.e. the TMD) and dissipating it in the damper. Maximum flow of energy from the primary system to the TMD occurs when the displacement of the TMD lags that of the primary mass by 90°. The acceleration of the TMD is then in phase with velocity of the primary system. The TMD concept was introduced by Frahm in 1909 to reduce the rolling motion of ships and ship hull vibrations. Significant theoretical contributions were made by Den Hartog (1940) for undamped systems subject to harmonic excitations. Extensions to the theory were then presented by Randall (1981), Warburton (1982) and Tsai & Lin (1993). The figure below illustrates the typical configuration of a unidirectional translational tuned mass damper. The mass rests on bearings that function as rollers and allow the mass to translate laterally relative to the floor. Springs and dampers are inserted between the mass and the adjacent vertical support members which transmit the lateral “outof-phase” force to the floor level, and then into the structural frame. Bidirectional translational dampers are configured with springs/dampers in 2 orthogonal directions and provide the capability for controlling structural motion in 2 orthogonal planes. The early versions of TMD’s employ complex mechanisms for the bearing and damping elements, have relatively large masses, occupy considerably space, and are quite expensive. Recent versions, such as the scheme shown below, have been designed to minimize these limitations. This scheme employs a multi-assemblage of elastomeric rubber bearings, which function as shear springs, and bitumen rubber compound (BRC) elements, which provide viscoelastic damping capability. The device is compact in size, requires unsophisticated controls, is multidirectional, and is easily assembled and modified. 845 Structural Engineering Analysis and Design Second Edition The problems associated with the bearings can be eliminated by supporting the mass with cables which allow the system to behave as a pendulum. The equation of motion for the horizontal direction is where T is the tension in the cable. When θ is small, the following approximations apply Hence and it follows that the equivalent shear spring stiffness is The natural frequency of the pendulum is The natural period of the pendulum is The simple pendulum tuned mass damper concept has a serious limitation. Since the period depends on L, the required length for large Td may be greater than the typical story height. This problem can be eliminated by resorting to the scheme illustrated below. 846 Structural Engineering Analysis and Design Second Edition The interior rigid link magnifies the support motion for the pendulum, and results in the following equilibrium equation. The rigid link moves in phase with the damper, and has the same displacement amplitude. Then, taking u1= ud The equivalent stiffness is Wd/2L, and it follows that the effective length is equal to 2L. Each additional link increases the effective length by L. The concepts of designing the passive tuned mass damper illustrated below are based on geometrically and materially linear frequency domain dynamic analyses. In deriving the equations of motion, we use absolute terms of displacement, velocity and acceleration unless we have support motion, in which case it is easier to use relative terms. Note that in absolute terms, we need the support displacement and velocity in the equation of motion whilst in relative terms we need only the support acceleration in the equation of motion. 847 Structural Engineering Analysis and Design Second Edition 5.6.4.1 Damped SDOF System Subject to Harmonic Force and Support Motion Excitations The analysis of the TMD involves the prediction of the response of a two-DOF system, the first being that of the primary system and the second being the TMD. Extensive use is made of (complex arithmetic) mathematical procedures to predict the steady-state response due to harmonic excitations in the frequency domain. The employment of complex arithmetic simply allows the representation of the response and the excitation functions in complex numbers. To illustrate this elegant mathematical approach, the steady-state response of a SDOF system is first illustrated, forming the basis of further analyses involving the TMD and the primary system. P(t) = p0cosωt k m cd & u&s ( t ) = a 0 cos ωt u(t) In absolute terms, the equation of motion of a SDOF system subjected to harmonic force excitation and support motion is m& u&( t ) + c(u&( t ) − u&s ( t ) ) + k (u ( t ) − u s ( t ) ) = P( t ) In relative terms, u r (t ) = u( t) − u s (t) Hence, m(& u&r ( t ) + & u&s ( t ) ) + cu&r ( t ) + ku r ( t ) = P( t ) m& u&r ( t ) + cu&r ( t ) + ku r ( t ) = P( t ) − m& u&s ( t ) For harmonic excitations, [ P( t ) = Re al p 0 e iωt ] and [ & u&s ( t ) = Re al a 0 e iωt ] [ ] For the inhomogenous part (steady - state solution), assume u r ( t ) = Re al F(ω)e iωt , − mω F(ω) + icωF(ω) + kF(ω) = p 0 + ma 0 2 F(ω) = F(ω) = F(ω) = p 0 + ma 0 k − mω 2 + icω p 0 + ma 0 (k − mω ) + (cω) e iθ 2 2 (1 − ω , θ = tan −1 2 (p 0 + ma 0 ) / k 2 / ωn ) 2 2 + (2ζω / ω n )2 2ζω / ω n cω = tan −1 2 k − mω 1 − ω2 / ωn 2 ( e −iθ , θ = tan −1 2ζω / ω n (1 − ω 2 / ωn 2 ) ) Thus, the steady - state solution is [ u r ( t ) = Re al F(ω)e iωt u r (t ) = (1 − ω ] (p 0 + ma 0 ) / k 2 / ωn ) 2 2 + (2ζω / ω n )2 cos(ωt − θ), θ = tan −1 848 2ζω / ω n (1 − ω 2 ω 2n ) Structural Engineering Analysis and Design Second Edition 5.6.4.2 Undamped Structure, Undamped TMD System Subject to Harmonic Force Excitation P(t) = p0cosωt k kd md m ud(t) u(t) ωn2 = k / m ωd2 = kd / md Note that In absolute terms, the equations of motion of the two − DOF system subjected to harmonic force excitation are m& u&( t ) + ku ( t ) − k d (u d ( t ) − u ( t ) ) = P( t ) md& u&d ( t ) + k d (u d ( t ) − u ( t ) ) = 0 For harmonic excitations, [ P( t ) = Re al p 0 e iωt ] [ ] [ ] For the inhomogenous part (steady - state solution), assume u ( t ) = Re al F(ω)e iωt and u d ( t ) = Re al Fd (ω)e iωt , − mω F(ω) + kF(ω) − k d Fd (ω) + k d F(ω) = p 0 2 − m d ω 2 Fd (ω) + k d Fd (ω) − k d F(ω) = 0 These are two equations which can be solved simultaneously for the complex frequency response functions (FRFs) F(ω) and Fd (ω) and converted into polar form to yield, F(ω) = ( ) p0 f 2 − ρ2 e iθ1 k 1 − ρ 2 f 2 − ρ 2 − µρ 2 f 2 Fd (ω) = [( )( ) ] p0 ρ e iθ 2 2 2 k 1 − ρ f − ρ 2 − µρ 2 f 2 2 [( )( ) ] Note that f = natural frequency ratio = ωd = ωn kd / md k/m ω ω ρ = forced frequency ratio = = ωn k/m m µ = mass ratio = d m For completion, the steady - state solutions are [ u ( t ) = Re al F(ω)e iωt [ u d ( t ) = Re al Fd (ω)e ] iωt ] The plot of the magnitude of the FRF F(ω) (of the primary system) divided by the static displacement p/k, i.e. the (magnitude of the) dynamic amplification factor D(ω) is presented. 849 Structural Engineering Analysis and Design Second Edition D(w) Dynamic Magnification Factor of Primary System D(w) 20 18 16 14 12 10 8 6 4 2 0 0.6 0.8 1 1.2 Forcing Frequency Ratio, ρ Primary Mass Primary Mass - TMD (f = 1.0) Primary Mass - TMD (f = 1.1) The optimum conditions are ascertained by changing the mass ratio µ and the natural frequency ratio f. Changing the frequency ratio, f has the effect of changing the position where D(ω) becomes zero, i.e. D(ω) becomes zero at when ρ = f. Changing the mass ratio has the effect of changing the distance between the peaks of D(ω) with higher values resulting in a greater spread. D(w) Dynamic Magnification Factor of Primary System D(w) 20 18 16 14 12 10 8 6 4 2 0 0.6 0.8 1 1.2 Forcing Frequency Ratio, ρ Primary Mass Primary Mass - TMD (mass ratio = 0.1) Primary Mass - TMD (mass ratio = 0.2) 850 Structural Engineering Analysis and Design Second Edition 5.6.4.3 Undamped Structure, Damped TMD System Subject to Harmonic Force Excitation P(t) = p0cosωt kd k m md cd ud(t) u(t) ωn2 = k / m ωd2 = kd / md c = 2ζωnm (here undefined) cd = 2ζdωdmd Note that In absolute terms, the equations of motion of the two − DOF system subjected to harmonic force excitation are m& u&( t ) + ku ( t ) − c d (u&d ( t ) − u&( t ) ) − k d (u d ( t ) − u ( t ) ) = P( t ) md& u&d ( t ) + c d (u&d ( t ) − u&( t ) ) + k d (u d ( t ) − u ( t ) ) = 0 For harmonic excitations, [ P( t ) = Re al p 0 e iωt ] [ ] [ ] For the inhomogenous part (steady - state solution), assume u ( t ) = Re al F(ω)e iωt and u d ( t ) = Re al Fd (ω)e iωt , − mω F(ω) + kF(ω) − ic d ωFd (ω) + ic d ωF(ω) − k d Fd (ω) + k d F(ω) = p 0 2 − m d ω 2 Fd (ω) + ic d ωFd (ω) − ic d ωF(ω) + k d Fd (ω) − k d F(ω) = 0 These are two equations which can be solved simultaneously for the complex frequency response functions (FRFs) F(ω) and Fd (ω) and converted into polar form to yield, F(ω) = p0 k Fd (ω) = (f − ρ ) + (2ζ ρf ) )(f − ρ ) − µρ f ] + [2ζ ρf [1 − ρ 2 [(1 − ρ p0 k 2 2 2 d 2 2 2 2 2 2 [(1 − ρ )(f 2 ρ 2 −ρ 2 ) − µρ f ] + [2ζ ρf [1 − ρ 2 2 2 d f = natural frequency ratio = ωd = ωn ρ = forced frequency ratio = ω = ωn k/m kd / md k/m ω md m For completion, the steady - state solutions are µ = mass ratio = u ( t ) = Re al F(ω)e iωt [ u d ( t ) = Re al Fd (ω)e ] iωt (1 + µ )]] 2 Note that [ 2 d e iθ1 2 ] 851 2 (1 + µ)]] 2 e iθ 2 Structural Engineering Analysis and Design Second Edition The plot of the magnitude of the FRF F(ω) (of the primary system) divided by the static displacement p/k, i.e. the (magnitude of the) dynamic amplification factor D(ω) is presented. D(w) Dynamic Magnification Factor of Primary System D(w) 20 18 16 14 12 10 8 6 4 2 0 Common Points 0.6 0.8 1 1.2 Forcing Frequency Ratio, ρ Damping 0.0 of Critical Damping 0.1 of Critical Damping 0.32 of Critical The optimum conditions are ascertained by changing the mass ratio µ, the natural frequency ratio f and the level of damping ζd. It is noticed that for whatever combination, there will always be two common points (which are independent of ζd) on the plot of D(ω). The greater the mass ratio µ, the lower will be the response. Also, a larger mass ratio would render the TMD less sensitive to tuning, a characteristic which is much valuable in practice as the estimate of the modal frequencies change with insertion of cladding, non-structural components etc. The mass ratio is usually between 0.01 and 0.1. By changing the ratio of the natural frequency ratio f, we will change the relative height of the two common points. The optimum condition will be when the two common points are at the same height. It can be shown from algebra that this condition is achieved when f is tuned such that f opt = 1 1+ µ which gives the amplitude at the common points as 2 D(ω) = 1 + µ By changing the damping ζd we will change the point at which the curves attain their maxima, i.e. whether at the above common points or not. We know that the amplitude at resonance is limited only by the damping force. If ζd = 0, there is no energy dissipation and hence two (since this is a two-DOF system) resonant peaks of infinite amplitude is attained on D(ω). When ζd is infinite, the two masses are practically locked to each other, their relative displacement is thus zero, hence causing no work to be done by the damper, and thus a single resonant peak of infinite amplitude is attained on D(ω). There is thus an optimum value of ζd for which there will be maximum work done by the damper, and this would be the point at which the response of the primary system is minimum. The 852 Structural Engineering Analysis and Design Second Edition optimum condition for the choice of ζd is achieved when the two curves pass the common points at the maxima. But this does not occur at the same time. Expressions for when the first curve passes the first common point at its maximum and the second curve passes the second common point at its maximum can be averaged to yield a useful optimum damping of ζ d ,opt = 3µ 8(1 + µ ) Thus, in order to design a TMD to reduce vibrations from harmonic force excitations, the following approach is undertaken. Clearly, one should select the TMD location to coincide with the maximum amplitude of the mode shape that is being controlled. (i) Choose the practically greatest possible mass ratio, µ whilst still satisfying the maximum displacement criteria for both F(ω) and Fd(ω) (ii) Determine the optimum natural frequency ratio, f and hence calculate the stiffness of the TMD, kd 1 f opt = 1+ µ ω d = f opt ω n k d = m d ω d2 (iii) Determine the optimum damping ratio, ζd,opt and hence calculate the optimum damping of the TMD, cd ζ d ,opt = 3µ 8(1 + µ ) c d ,opt = 2ζ d ,opt ω d m d As an example, we shall investigate the design of a TMD for the London Heathrow Terminal 5 Visual Control Tower. The 85.5m high tower has a total mass of 680.9 tonnes and a fundamental global tower mode (0.91Hz) modal mass of 396 tonnes with the eigenvector normalized at the location of the TMD, i.e. at 78.3m. Note that there are other local (cable) modes of lower frequencies. 853 Structural Engineering Analysis and Design Second Edition The natural frequencies of the modes of the tower are presented for completion. The corresponding modal masses are also presented with the eigenvectors MAX normalized. T5 VCR REAL MODAL ANALYSIS - FREQUENCY 4.000 Cable Modes 3.500 Secondary Tower Bending Modes Frequency (Hz) 3.000 2.500 Cable Modes 2.000 Primary Tower Torsion Mode Cable Modes 1.500 Cable Modes 1.000 Primary Tower Bending Modes 0.500 0.000 0 5 10 15 20 25 30 35 40 45 50 Mode Number T5 VCR REAL MODAL ANALYSIS - MODAL MASS 250.000 S econdary Tower Bending Modes 225.000 Modal Mass (Tonnes) 200.000 175.000 150.000 Primary Tower Torsion Mode Primary Tower Bending Modes 125.000 100.000 75.000 50.000 Cable Modes Cable Modes Cable Modes Cable Modes 25.000 0.000 0 5 10 15 20 25 30 Mode Number 854 35 40 45 50 Structural Engineering Analysis and Design Second Edition Natural Frequency (Hz) The characteristic of the modes are also expounded. The calculation for optimum properties of a 25 tonne TMD is presented. md 25000 = = 0.0631 m 396000 1 Optimum Frequency Ratio, f opt = = 0.9406 1+ µ Frequency of Secondary System, f d = f opt f 1 Mass Ratio, µ = = 0.9406 * 0.951 = 0.895 Hz Optimum Stiffness of TMD, k d = m d (2πf d ) 2 = 25000 * (2π * 0.895 )2 = 789745.14 N/m Optimum Damping Ratio, ζ opt = 3µ 8(1 + µ) = 0.14922 Viscous Damping Coefficient, c d = 2m d ω d ζ opt = 2 * 25000 * (2πf d )ζ opt = 41936.103 Ns/m 855 Structural Engineering Analysis and Design Second Edition The figure below shows the displacement magnification factor D(ω) at the AMD level with harmonic excitation at the AMD level. This shows that the effective damping of the primary tower mode from the TMD is 9.7% of critical since the reduction of maximum amplification reduces from 33.2 to 4.84. 856 Structural Engineering Analysis and Design Second Edition 5.6.4.4 Undamped Structure, Damped TMD System Subject to Harmonic Support Motion kd k m md cd ud(t) u(t) üs(t) = a0cosωt In absolute terms, the equations of motion of the two − DOF system subjected to harmonic support motion are m& u&( t ) + k (u ( t ) − u s ( t ) ) − c d (u&d ( t ) − u&( t ) ) − k d (u d ( t ) − u ( t ) ) = 0 md& u&d ( t ) + c d (u&d ( t ) − u&( t ) ) + k d (u d ( t ) − u ( t ) ) = 0 In relative terms, u r (t ) = u( t) − u s (t ) u dr ( t ) = u d ( t ) − u ( t ) = u d ( t ) − u r ( t ) − u s ( t ) Hence, m& u&r ( t ) + ku r ( t ) − c d u&dr ( t ) − k d u dr ( t ) = −m& u&s ( t ) md& u&dr ( t ) + c d u&dr ( t ) + k d u dr ( t ) = −m d & u&s ( t ) − m d & u&r ( t ) For harmonic excitations, [ & u&s ( t ) = Re al a 0 e iωt ] [ ] [ ] For the inhomogenous part (steady - state solution), assume u r ( t ) = Re al F(ω)e iωt and u dr ( t ) = Re al Fd (ω)e iωt , −mω F(ω) + kF(ω) − ic d ωFd (ω) − k d Fd (ω) = −ma 0 2 −m d ω 2 Fd (ω) + ic d ωFd (ω) + k d Fd (ω) = −m d a 0 + m d ω 2 F(ω) These are two equations which can be solved simultaneously for the complex frequency response functions (FRFs) F(ω) and Fd (ω) and converted into polar form to yield, F(ω) = − Fd (ω) = − [(1 + µ)f − ρ ] + (2ζ ρf (1 + µ)) )(f − ρ ) − µρ f ] + [2ζ ρf [1 − ρ 2 2 2 a 0m k [(1 − ρ a 0m k 2 d 2 2 2 2 2 2 [(1 − ρ )(f 2 (1 + µ )]] 1 2 −ρ 2 ) − µρ f ] + [2ζ ρf [1 − ρ 2 2 2 d Note that f = natural frequency ratio = ωd = ωn ρ = forced frequency ratio = ω = ωn k/m kd / md k/m ω md m For completion, the steady - state solutions are µ = mass ratio = [ ] ( t ) = Re al [F (ω)e ] u r ( t ) = Re al F(ω)e iωt u dr 2 d iωt d 857 e iθ3 2 2 (1 + µ )]] 2 e iθ 4 Structural Engineering Analysis and Design Second Edition The amplification factors for harmonic ground motion are essentially similar to the amplification factors for external harmonic loading so long as the mass ratio is small. The exact expressions for the optimum conditions for harmonic ground motion are nevertheless presented here. As before, the optimum conditions are ascertained by changing the mass ratio µ, the forcing frequency ratio f and the level of damping ζd. It is noticed that for whatever combination, there will always be two common points (which are independent of ζd) on the plot of D(ω). The greater the mass ratio, the lower will be the response. The mass ratio is usually between 0.01 and 0.1. By changing the ratio of the forcing frequency f, we will change the relative height of the two common points. The optimum condition will be when the two common points are at the same height. The optimum frequency ratio f is f opt = 1− µ/ 2 1+ µ The optimum condition for the choice of ζd is achieved when the two curves pass the common points at the maxima. But this does not occur at the same time. An average damping ratio that yields the optimum damping is ζ d ,opt = 3µ 8(1 + µ )(1 − µ / 2 ) Thus, in order to design a TMD to reduce vibrations from harmonic force excitations, the following approach is undertaken. Clearly, one should select the TMD location to coincide with the maximum amplitude of the mode shape that is being controlled. (i) Choose the practically greatest possible mass ratio, µ whilst still satisfying the maximum displacement criteria for both F(ω) and Fd(ω) (ii) Determine the optimum natural frequency ratio, f and hence calculate the stiffness of the TMD, kd 1− µ / 2 1+ µ ω d = f opt ω n f opt = k d = m d ω d2 (iii) Determine the optimum damping ratio, ζd,opt and hence calculate the optimum damping of the TMD, cd ζ d ,opt = 3µ 8(1 + µ )(1 − µ / 2 ) c d ,opt = 2ζ d ,opt ω d m d 858 Structural Engineering Analysis and Design Second Edition 5.6.4.5 Damped Structure, Damped TMD System Subject to Harmonic Force and Support Motion P(t) = p0cosωt kd k m c md cd ud(t) u(t) üs(t) = a0cosωt In absolute terms, the equations of motion of the two − DOF system subjected to harmonic force and support motion are m& u&( t ) + c(u&( t ) − u&s ( t ) ) + k (u ( t ) − u s ( t ) ) − c d (u&d ( t ) − u&( t ) ) − k d (u d ( t ) − u ( t ) ) = P( t ) md& u&d ( t ) + c d (u&d ( t ) − u&( t ) ) + k d (u d ( t ) − u ( t ) ) = 0 In relative terms, u r (t ) = u (t) − u s (t ) u dr ( t ) = u d ( t ) − u ( t ) = u d ( t ) − u r ( t ) − u s ( t ) Hence, m& u&r ( t ) + cu&r ( t ) + ku r ( t ) − c d u&dr ( t ) − k d u dr ( t ) = P( t ) − m& u&s ( t ) md& u&dr ( t ) + c d u&dr ( t ) + k d u dr ( t ) = −m d & u&s ( t ) − m d & u&r ( t ) For harmonic excitations, [ P( t ) = Re al p 0 e iωt ] [ & u&s ( t ) = Re al a 0 e iωt and ] [ ] [ ] For the inhomogenous part (steady - state solution), assume u r ( t ) = Re al F(ω)e iωt and u dr ( t ) = Re al Fd (ω)e iωt , −mω F(ω) + icωF(ω) + kF(ω) − ic d ωFd (ω) − k d Fd (ω) = p 0 − ma 0 2 −m d ω 2 Fd (ω) + ic d ωFd (ω) + k d Fd (ω) = −m d a 0 + m d ω 2 F(ω) These are two equations which can be solved simultaneously for the complex frequency response functions (FRFs) F(ω) and Fd (ω) and converted into polar form to yield, F(ω) = ( ) ] f 2 − ρ 2 + (2ζ d ρf )2 p0 e iθ1 k − f 2 ρ 2 µ + 1 − ρ 2 f 2 − ρ 2 − 4ζζ fρ 2 2 + 4 ζρ f 2 − ρ 2 + ζ fρ 1 − ρ 2 (1 + µ ) 2  d d   [ ( )( ) [ 2 ( [ ) ] ] ] (1 + µ )f 2 − ρ 2 + (2ζ d ρf (1 + µ ))2 a m − 0 e iθ 2 k − f 2 ρ 2 µ + 1 − ρ 2 f 2 − ρ 2 − 4ζζ fρ 2 2 + 4 ζρ f 2 − ρ 2 + ζ fρ 1 − ρ 2 (1 + µ ) 2  d d   2 p ρ Fd (ω) = 0 e iθ3 2 2 2 2 2 2 2 2 2 2 2 k − f ρ µ + 1 − ρ f − ρ − 4ζζ fρ + 4 ζρ f − ρ + ζ d fρ 1 − ρ (1 + µ )  d   a m 1 − 0 e iθ 4 2 2 2 2 2 2 2 2 2 2 2 k − f ρ µ + 1 − ρ f − ρ − 4ζζ fρ + 4 ζρ f − ρ + ζ d fρ 1 − ρ (1 + µ )  d   For completion, the steady - state solutions are [ ( [ ( [ )( )( ( 2 ) ] ) )( [ ] ( t ) = Re al [F (ω)e ] u r ( t ) = Re al F(ω)e iωt u dr ( ] ) iωt d 859 ( [ ) ( [ ) ) ] ] [ ] Structural Engineering Analysis and Design Second Edition As before, the optimum conditions are ascertained by changing the mass ratio µ, the forcing frequency ratio f and the level of damping ζd. The greater the mass ratio, the lower will be the response. The mass ratio is usually between 0.01 and 0.1. Analytical solutions for the optimum natural frequency ratio, f and the optimum damping ratio, ζd,opt cannot be found. The two common points (which are independent of ζd) on the D(ω) plot no longer exist. For force excitation, the optimum values of f and ζd for small values of ζ can be formulated empirically (Ioi and Ikeda, 1978) as follows. 1 f opt = − (0.241 + 1.7µ − 2.6µ 2 )ζ − (1.0 − 1.9µ + µ 2 )ζ 2 1+ µ 3µ + (0.13 + 0.12µ + 0.4µ 2 )ζ − (0.01 + 0.9µ + 3µ 2 )ζ 2 8(1 + µ ) Tolerance or permissible error ranges attached to the above equations are found to be less than 1% for 0.03 < µ < 0.40 and 0.0 < ζ < 0.15, which are the ranges of practical interest. ζd = 860 Structural Engineering Analysis and Design Second Edition 5.6.4.6 TMD Analysis Summary (Warburton, 1982) Clearly, one should select the TMD location to coincide with the maximum amplitude of the mode shape that is being controlled. The mass of the primary system will be the (POINT normalized to the TMD DOF) modal mass of the mode in which damping is intended. The greater the mass ratio µ, the lower will be the response and the smaller the sensitivity to tuning. Hence, choose the practically greatest possible mass ratio, µ whilst still satisfying the maximum displacement criteria for both F(ω) and Fd(ω). Then determine the optimum natural frequency ratio, f and hence calculate the stiffness of the TMD, kd = mdωd2. Finally, determine the optimum damping ratio, ζd,opt and hence calculate the optimum damping of the TMD, cd = 2ζd,optωdmd. The structure and the TMD can be modeled and analyzed within a MSC.NASTRAN frequency domain analysis (SOL 108 or SOL 112) to confirm the results. System Damped System Undamped System, Undamped TMD Undamped System, Damped TMD Undamped System, Damped TMD Undamped System, Damped TMD Undamped System, Damped TMD Undamped System, Damped TMD Undamped System, Damped TMD Damped System, Damped TMD Damped System, Damped TMD Optimized Parameter Optimum Natural Frequency Ratio, fopt = ωd/ωn Optimum TMD Damping, ζd,opt Primary Mass and Support Primary Mass Displacement N/A N/A Deterministic Harmonic Primary Mass Primary Mass Displacement N/A N/A Deterministic Harmonic Primary Mass Primary Mass Displacement 1 1+ µ 3µ 8(1 + µ ) Deterministic Harmonic Primary Mass Primary Mass Acceleration 1 1+ µ 3µ 8(1 + µ / 2 ) Deterministic Harmonic Support Primary Mass Displacement 1− µ / 2 1+ µ 3µ 8(1 + µ )(1 − µ / 2 ) Deterministic Harmonic Support Primary Mass Acceleration Random Primary Mass Excitation Type Excitation Applied To Deterministic Harmonic Random Deterministic Harmonic 1 1+ µ 1+ µ / 2 1+ µ 1− µ / 2 1+ µ Support Primary Mass Primary Mass Displacement 1 1+ µ Primary Mass Primary Mass Displacement 0.0 p0 2 1+ k µ p0 k 2 µ(1 + µ) ma 0 2 (1 + µ) k µ ma 0 k 1+ 2 µ 1 + 3µ / 4 µ(1 + µ) µ(1 − µ / 4) 4(1 + µ )(1 − µ / 2 ) ma 0 (1 + µ) 1.5 . k 1 1 − µ 4 3µ 8(1 + µ ) + (0.13 + 0.12µ + 0.4µ 2 )ζ − (0.01 + 0.9µ + 3µ 2 )ζ 2 3µ(1 + 0.49µ − 0.2µ 2 ) 8(1 + µ ) + (0.096 + 0.88µ − 1.8µ 2 )ζ + (0.13 + 0.72µ + 0.2µ 2 )ζ + (1.34 − 2.9µ + 3µ 2 )ζ 2 + (0.19 + 1.6µ − 4µ 2 )ζ 2 861 ) p0 k − (1.0 − 1.9µ + µ 2 )ζ 2 1+ µ ( 2ζ 1 − ζ 2 µ(1 + 3µ / 4) 4(1 + µ )(1 + µ / 2 ) − (0.241 + 1.7µ − 2.6µ 2 )ζ 1 Deterministic Harmonic 3µ 8(1 + µ ) Optimized Maximum (Relative) Response of Structure, ur (p 0 + ma 0 ) / k Structural Engineering Analysis and Design Second Edition The displacement optimization parameter is used essentially to determine the safety and integrity of the structure under external excitations. Since large accelerations of a structure under excitations produce detrimental effects on functionality of nonstructural components, base shear and occupant comfort, minimizing structural accelerations can also be a viable optimization criterion. The effective damping often quoted for a system with a TMD is obtained simply by the following equation ζeff = 1/(2Dopt(ω)) as this is consistent with the definition of the maximum dynamic amplification for SDOF systems without TMD which for small values of ζ is Dmax(ω) = 1/(2ζ) For broadband seismic applications, Villaverde (1985) had suggested the following equations for optimum parameters with mass ratio based on modal mass with eigenvector POINT normalized to location of TMD. f opt = 1 ζ d ,opt = ζ + µ For broadband seismic applications, Fadek et. al. (1997) suggested the following equations for optimum parameters with mass ratio based on modal mass with eigenvector POINT normalized to location of TMD. 1  µ  f opt = 1 − ζ  1 + µ  1 + µ  ζ d ,opt = ζ µ + 1+ µ 1+ µ TMD are effective in seismic applications for structures with low damping, ζ = 0.02. For structures with damping, ζ = 0.05, TMDs are not very effective since a very large mass ratio is required. TMDs are also not effective in seismic applications of very stiff structures with periods 0.1-0.2s. 862 Structural Engineering Analysis and Design Second Edition GL, ML Tuned Slosh Damper (TSD) Systems 16 5.6.5 TSDs can, in some cases, present a cost-effective alternative to Tuned Mass Dampers for reducing the response of lively structures. Their principle strengths are low initial cost and virtually maintenance-free operation. 5.6.5.1 When To Employ TSDs For a TSD to be the right solution, the following should be true: I. II. III. The problem motion of the structure is predominantly horizontal at the proposed location of the damper. The volume available for the damper is at least twice that of the TSD liquid which would provide the required damper mass. This allows space for sloshing and the redundant mass of liquid. The problem mode has a natural frequency below 2 Hz. Above this frequency, dampers become so small that a prohibitively large number of damper tanks would be necessary to generate appreciable damper mass. Number of damper tanks required for a 1 tonne damper Number of Damper Tanks 2000 1500 1000 500 0 0 0.5 1 1.5 2 Design Frequency /Hz The following is desirable: I. 5.6.5.2 The natural frequency of the problem mode is accurately known (i.e. from testing). TSDs can be designed to work across a range of natural frequency however, this can lead to increasing the complexity of the design, having a variable damper mass or reducing the effectiveness of the damper for low amplitude motions. The concession is dependent on the design route taken. Operations of TSDs Broadly speaking, two types of TSD have been fitted to structures: I. 16 ‘Shallow tanks’ where the water height to length ratio is less than 0.1 and the damping is governed chiefly by wave breaking and viscous action. POWELL, Daniel. Tuned Slosh Dampers. Ove Arup & Partners Ltd., London, 2003. 863 Structural Engineering Analysis and Design Second Edition II. ‘Deep tanks’ where the damping is generated by resistance elements in the centre of the tank applying drag forces to the sloshing liquid These two types of damper can be implemented in either rectangular or cylindrical tanks. If a structure is susceptible to lateral excitation in two perpendicular directions, it is possible to use a rectangular damper with matching sloshing frequencies in the relevant directions. More often than not, the liquid used in TSDs is water, the main reason for this being cost. 5.6.5.2.1 Sloshing Frequency Damping elements (Deep Tank only) undisturbed liquid level h a Excitation The sloshing frequency of the nth mode of the tank geometry shown above is given by fn = 1 ng  nπh  tanh  2 πa  a  Note that I. The only modes of practical interest are the first two asymmetric modes i.e. n=1 the fundamental sloshing frequency which is tuned to the structure and, to a lesser extent, n=3 (the mass of liquid associated with this mode is much lower). II. A tank of length ‘a’ has a maximum fundamental natural frequency given by 1 g i.e. this 2 πa frequency can’t be exceeded by raising h. In practice, for a given damper arrangement, the TSD damping decreases with increasing h/a and it is unlikely you would choose to have this ratio greater than 0.4. Note that h/a ratios of 0.1 to 0.35 are typical for a deep tank damper. III. The sloshing frequency’s sensitivity to changes in ‘h’ is greatest when h is small hence, if a fixedlength shallow tank damper is designed for a structure whose natural frequency is slightly different from that predicted, the effective mass of the re-tuned damper can be very different from the design value. IV. This formula is developed using linear theory and the frequencies it predicts are for the related sloshing modes i.e. for the fundamental mode the liquid surface is approximately a cosine between 0 and π. For shallow tanks, and deep tanks under large amplitude excitation, other sloshing modes will become apparent. 864 Structural Engineering Analysis and Design Second Edition 5.6.5.2.2 Effective Mass and “Housner” Respresentation Not all the liquid in a TSD takes part in the fundamental sloshing mode. There is a fraction, typically 20-30% in deep tanks and <10% in shallow tanks, which can be considered as static mass added to the structure. The rest of the liquid is actively sloshing and the mass of this liquid (the ‘effective mass’) can be thought of as that equivalent to the mass in a TMD. An equivalent mechanical representation of liquid sloshing in tanks was developed by Housner in the 1950s and is illustrated below. Housner representation of horizontally excited liquid in tank a M1 h M0 h1 h0 M.g where effective mass M1 a  πh  = 0.527 tanh  M 2h  a  (b is the damper tank’s internal breadth) static mass M 0 = M − M1 height of effective mass  πh  cosh  − 2 h1  a  = 1− πh h  πh  sinh   a  a  height of static mass   h0 1  4 =  h 8    tanh  3a   2h        − 1 3a   2h By evaluating the fundamental sloshing frequency from fn = 1 ng  nπh  tanh  2 πa  a  the equivalent spring coefficient can be calculated for the Housner model using f = 1 2π k . The heights of the M1 effective and redundant mass give the dynamic moments about the base of the damper due to the ‘spring’ force and 865 Structural Engineering Analysis and Design Second Edition inertia force, respectively. The values of these heights could be considered counter-intuitive, it is not unusual for both values to be greater than h, particularly for shallower tanks. For deeper tanks h0 and h1 can be almost equal. 5.6.5.2.3 Sloshing Height As part of the TSD design process it is necessary to estimate the sloshing height of the damper. Warnitchai and Pinkaew’s (Engineering Structures Vol. 20 No. 7) method requires the iterative solving of an equation, Housner’s method is more straight-forward but its form causes stability problems in an iterative spreadsheet, as is required for evaluating the non-linear damping of a TSD. Another, simpler, method for estimating the sloshing height for deep tank TSD is presented. The two basic assumptions are: I. The liquid surface is a half cosine wave. II. The displacement of the centre of mass of the sloshing liquid is equal to the displacement of the mass in an equivalent TMD. Clearly this second assumption is a little simplistic as different regions of the TSD liquid move at different rates, however, following these assumptions leads to the following expression: - Λ≈ where: - hπ 2 d tmd 2a is sloshing height above undisturbed liquid level is displacement of an equivalent TMD Better agreement between this formula and Housner’s method is achieved if a ‘fudge-factor’ of 0.75 is applied to the above expression. Λ d tmd Λ ≈ 0.75 hπ 2 d tmd 2a To calculate the equivalent TMD performance, the damping of the TSD needs to be calculated (which in turn being response dependent requires the sloshing height, hence the requirement for an iterative spreadsheet). 5.6.5.2.4 Stoke’s Number and Nonlinear Sloshing Under modest levels of excitation, a TSD will slosh in the linear manner discussed previously with fundamental natural frequency and effective mass close to values obtained from the formulae listed. At higher levels of excitation sloshing non-linearities are present and new modes appear. There is also a new source of damping through wave breaking. The transition from the linear state occurs at much lower levels of excitation in a shallow tank damper. The parameter which governs the degree of non-linearity of sloshing of a TSD is the Stokes' Number, Us. Us = 4 Λa 2 h3 At low values of Us (say <20), the TSD sloshing is close to linear. The principle deviation from linear behaviour, in this Us range, being that the low-level and high-level sloshing heights are not of equal magnitude, the high-level is around 30% greater at a Us of 10. Despite this, the formulae listed previously based on a linear model still hold. If damping elements are not present to apply drag-forces on the fluid, damping is very low in this regime of Us (typically <0.5%). As Us increases, the asymmetry about the undisturbed water height becomes more pronounced and additional sloshing modes become apparent. Also, wave breaking becomes a significant source of damping. In this non-linear sloshing regime, the importance of accurate tuning of the damper reduces and the eventually device becomes more passive-energy-dissipater than tuned-vibration absorber. 5.6.5.2.5 Damping in TSDs Damping is chiefly introduced by two different mechanisms in TSDs: I. Damping elements applying drag forces – obstructions fixed in the tank impede the sloshing of the liquid. 866 Structural Engineering Analysis and Design Second Edition II. Wave breaking – at high Stokes' Numbers (i.e. in deep tank dampers under high amplitudes of excitation and shallow tank dampers generally) significant wave breaking occurs which dissipates energy. Damping Elements Damping elements are obstructions immersed in the TSD liquid which the liquid flows past while sloshing. Drag forces are applied by the damping elements on the liquid, this introduces damping into the system. Damping elements are normally located in the centre of the tank where the peak velocity of the liquid is a maximum. Typically damping elements obstruct around 25% of the flow area though this is dependent on the level of damping required. Frequently used designs of damping element include baffles normal to the flow, perforated plates and wire-mesh screens. The drag forces objects immersed in fluids, can be thought of as being comprised of two parts: Skin-friction Dτ – the forces applied by shearing as the liquid passes the solid boundaries. Pressure-drag DP – the net forces applied to the body due to differences in the upstream and downstream pressure fields. Broadly speaking, both components of the total drag force increase with fluid velocity V. where n is in the range 1.2 → 1.8 Dτ ∝ Vn DP ∝ V2 The relative magnitude of these two drag components depends on the geometry of the object in the fluid. For ‘stream-lined’ bodies e.g. a flat plate parallel to the flow direction, the drag will be almost entirely skin friction while for ‘bluff’ bodies e.g. a flat plate normal to the flow direction, the pressure drag will dominate. For some cross-sections e.g. a cylinder, the ratio of these two drag forces varies considerably depending on the flow regime and these simple relationships between drag and fluid velocity are of limited use. The reason the composition of the drag forces on the damping elements is significant, is that this governs the degree of non-linearity of the TSD damping. If the drag on the damping elements is mainly viscous and the value of n in the expression above is close to 1 then the damping in the TSD is close to linear i.e. the damping ratio is approximately constant. On the other hand, if the damping elements are such that the force on them is dominated by the pressure-drag component e.g. baffles normal to the flow, the damping is non-linear and amplitude dependent. Realistically, damping elements which provide predominantly viscous drag across a wide range of Re e.g. baffles parallel to the flow, are unlikely to provide sufficient total drag for the damping required in a TSD. One approach is to use a very fine mesh of wires with cylindrical cross-section such that Re number remains low (say up to 2) during sloshing. One practical concern with this design is that the mesh will clog up very easily, this would change the blockage ratio and consequently the performance of the damper. Warnitchai and Pinkaew developed an equation suggesting that for damping elements of constant CD, the damping ratio of a TSD is directly proportional to the sloshing height, Λ. This linear relationship is verified by experiment however, the quantitative predictions from the equation are poor if realistic values for CD are substituted into the expression, the damping levels predicted being far too low. Flat plates normal to flow have a drag coefficient which is approximately constant across a wide range of Re. This is because of the small proportion of surface area in the flow-wise direction for the liquid to shear against, also the point at which fluid passing the plate separates from the surface (i.e. the edges of the plate) is independent of Re, meaning the wake area (area over which pressure-drag acts) at the rear of the plate will remain constant. Hence the drag is dominated by the pressure-drag and increases with V2. Therefore, if baffles normal to the sloshing direction are used as damping elements, the TSD damping is approximately proportional to sloshing height. Thus, this type of damping element produces very low damping levels at very low amplitudes of excitation. 867 Structural Engineering Analysis and Design Second Edition Based on the proportionality relationship developed by Warnitchai and Pinkaew, an empirical formula is developed to estimate the TSD damping in a deep tank damper for damping elements of constant drag coefficient. ε TSD = ε 0 + K.Λ where ε0 is the damping if the TSD has no damping elements i.e. damping due to shearing at the edge of the tank between the tank surfaces and the liquid. The value of this damping offset for deep tank TSDs with length to breadth ratio of about two is typically 0.3→0.4%. As this damping is due purely to shear, it has a low dependence on the sloshing height, Λ. The above equation is not valid for all values of Λ, for large sloshing heights and hence Stokes’ Numbers, the damping will be supplemented by wave breaking and the relationship will no longer be linear. K is a constant dependent on the drag coefficient, blockage ratio and h/a ratio of the TSD. Its value can be obtained by calculating the gradient on a plot of damping against sloshing height. Damping element details of the figure above Case (a) - No Damping Elements (εTSD= ε0) Case (b) - two cylinders of diameter 22 mm (blockage, Ø = 0.22) Case (c) - 50 mm flat plate normal to sloshing (Ø = 0.25) Case (d) - mesh screen, wire diameter 0.26 mm (Ø = 0.29) Some tabulated K values are as follows. Style of Damping Element Blockage Ratio h/a (TSD height/length) 868 K /m -1 Structural Engineering Analysis and Design Second Edition vertical cylinders 0.22 0.3 0.33 Baffles normal 0.25 0.3 1.80 “ 0.17 0.4 1.31 “ 0.25 0.4 1.65 “ 0.33 0.4 2.39 to flow For three cases, the trend is for a straight line crossing the y-axis at ε0 (~0.003 in this case) the exception is case (d). For this case the y-axis is intersected at a significantly higher value and there is a less obvious linear fit to the data. One might expect cases (b) and (d) to exhibit similar trends, both damping elements consisting essentially of flow obstructions of circular cross-section. The difference lies in the Re numbers. The Re number of the flow past damping elements varies between zero, when the liquid is instantaneously stationary at the extremity of sloshing, and some maximum value, a quarter of a sloshing cycle later, when the liquid surface is nominally flat and the velocity across the damping elements a maximum. The characteristic dimensions for the calculation of Re number in cases (b) and (d) are 22 and 0.26 mm, respectively. Consequently, for a sloshing height of 2 cm, the corresponding theoretical maximum Re numbers are 350 and 4. Inspection of the CD versus Re figure indicates that the drag coefficients in the two TSDs vary across very different ranges, hence drag forces and consequently damping characteristics are very different. In order to calculate Re numbers in a TSD, an estimate of the liquid speed at the centre of the tank is required. A velocity potential function for the liquid is derived in Warnitchai and Pinkaew based on linear theory and, hence, only applicable to deep tank dampers. By differentiating this expression with respect to the spatial coordinate in the sloshing direction (x), an expression for the liquid velocity is obtained, dependent on time and position in the tank. Substituting in the x value for the mid-point of the tank yields: -  π ( z + h)  cosh   a   . sin( 2πf t ) U x = Λ. 1 π h   sinh    a  where the previously defined symbols have the same meanings and: - Ux z f1 t is the liquid velocity in the horizontal sloshing direction / m/s is the vertical co-ordinate with origin at the undisturbed liquid surface / m is the fundamental sloshing mode of the TSD / Hz is time / s For a given Λ , h and a, the magnitude of U x will be a maximum when sin( 2πf 1t ) =1. If this is substituted into the above equation, the result is a profile of U x magnitudes against z which can be integrated up to obtain a mean value of U x , U x where: - Ux = Λa πh This is the magnitude of a sinusoid so a more representative value is the RMS of this i.e.: - U x RMS = Λa πh 2 This equation can be used to generate the velocity term when calculating practical values of Re number for the flow across damping elements. Establishing the Re number for damping elements of circular section helps give a 869 Structural Engineering Analysis and Design Second Edition qualitative prediction of their behaviour. If the Re number is very low e.g. < 2, the drag will have a significant viscous component and the TSD will have useful damping at very low levels of excitation (e.g. 2 cm sloshing height for a typical deep tank TSD) and the TSD’s damping will have less dependence on sloshing height. If however the Re number is larger than 100, the drag will be dominated by the pressure-drag and, for all practical Re numbers, the drag coefficient will be approximately constant (assuming the Re Number isn’t going to exceed 105 !), consequently, the TSD damping will be approximately proportional to sloshing height. As all TSDs with practical damping levels exhibit some dependence on response, the damping ratio will fall-off either side of resonance as the magnification factor reduces. Wave Breaking At higher Stokes’ Numbers (i.e. high amplitudes of excitation), surface tension is no longer strong enough to keep the liquid surface continuous and ‘wave breaking’ occurs. There are significant losses associated with this process which introduce additional damping into the system. In this sloshing regime, the TSDs behaviour deviates significantly from the linear models used to represent lower amplitude excitation and it is no longer valid to use them. In our existing TSD literature, there is no method presented for predicting the damping due to wave breaking and. Typically dampers of 1 to 1.5% of the modal mass of a lightly damped structure can increase the effective structural damping to between 4 and 5%. One of the main advantages of TSDs which rely on wave breaking to provide the damping is that the performance of the damper is relatively insensitive to tuning ratio. 5.6.5.2.6 Conditions at Resonance As for all resonant systems with damping, TSDs exhibit a frequency shift such that the maximum magnification factor (and hence maximum sloshing height in a ‘frequency-sweep’ test) occurs at tuning-ratios of less than 1, where tuning ratio is defined as: - r= where fe f1 fe f1 is excitation frequency /Hz and is the fundamental sloshing frequency The tuning ratio where the resonance occurs in conventional TMDs is given by: - r = 1 − 2ε 2 where ε is the damping ratio. For the case of deep tank TSDs with damping elements, an additional frequency shift occurs. This can be qualitatively explains as follows: - the liquid flow past the damping elements is unsteady and continuously accelerating and decelerating. To drive these changes in velocity (by Newton’s Second Law) a variable pressure gradient must exist in the liquid. As the damping elements are immersed in the liquid, they experience a force due to this pressure gradient (as described in ‘Morison’s Equation’) and consequently react a drag force back onto the liquid. This drag-force is conservative (as it is transferring momentum elastically between TSD liquid and structure) and introduces no damping yet, as it is applying a force on the liquid, it is responsible for a reduction in natural frequency. The frequency shift due to this effect is calculated analytically in Warnitchai and Pinkaew. However, in tests this theoretical treatment was found to over-predict the magnitude of the frequency reduction. From the tests carried out on the Arup Gatwick project, 2% was found to be a practical reduction in the TSD fundamental frequency. This factor allows for both the reduction due to damping and blockage. This figure was seen to be approximately correct for damping ratios of order 5-10% and blockage ratios from 0.15-0.35. The frequency at which the maximum lateral force exerted by the tank on the structure occurs does not necessarily correspond with the frequency of maximum sloshing height. Indeed, dependent on the size of the redundant liquid mass and the mass of the empty tank, the frequency of maximum lateral force can be higher or lower than f 1 . 870 Structural Engineering Analysis and Design Second Edition 5.6.5.3 Deep or Shallow Tank? As previously discussed, TSDs can be thought of as being shallow tank (h/a<≈0.1) or deep tank. 5.6.5.3.1 Deep Tank Performance can be predicted analytically – as have been discussed, analytical methods exist for predicting the behaviour of deep tank dampers. Given the cost of testing TSDs, this is a considerable asset. High mass – although the proportion of liquid which contributes to the sloshing (effective mass) increases as a damper is made shallower, the absolute effective mass decreases. Thus, achieving the same mass ratio between structure and damper with shallow tanks requires more tanks and, in all likelihood, more complexity, as dampers might need to be stacked. 5.6.5.3.2 Shallow Tank Relatively insensitive to tuning ratio – as the sloshing of a shallow tank damper is non-linear, the Housner representation is not a good representation of the behaviour. Shallow tank dampers act more as passive energy absorbers than TMDs or deep tank TSDs, consequently they reduce the worst-case response to a lesser extent than a well-tuned TMD but they achieve a useful reduction across a broad range of tuning ratios. 5.6.5.3.3 Practical Considerations Due to the relatively low mass of a shallow tank damper, many tanks are usually required to achieve the required damper to structure ratio. Hence this style of TSD lends itself to prefabricated stacks of dampers which can be fixed to a supporting frame on the structure (see reference 1 for examples of this). Once fabricated the only option available for tuning the frequency of the dampers is adjusting the water depth. Thus, if the natural frequency of the structure is not known accurately prior to design (i.e. has not been measured), the effective mass and mass ratio of the dampers can vary significantly. For the case of deep tank TSDs, it is more probable that the damper mass will be provided by a small number of large tanks. It is therefore likely that it will be practical to install an adjustable baffle within each of the tanks allowing variation of the damper dimension in the sloshing direction. This allows greater control of the effective mass of the TSDs across a range of frequencies, as when a reduction in TSD design frequency is required, the reduction in depth can be accompanied/replaced by an increase in length (the converse is also true but it is unlikely that the damper being too massive would be a problem). In summary, a shallow tank TSD has desirable characteristics if the in-service frequency of the structure is likely to vary (say +/- 5%) about some well-defined initial value, while a deep tank TSD might be the preferred option if the frequency is not likely to vary significantly in service (though this might be allowed for by ‘spread-tuning’). If the design of the TSD is developing in tandem with the structure, deep tank TSDs are probably the more sensible option as it’s more likely their design-frequency can be changed without compromising their performance. 871 Structural Engineering Analysis and Design Second Edition 5.6.5.4 Testing 5.6.5.4.1 Experimental Set-Up In order to test the performance of a TSD, a device is required to replicate the lateral motions of the structure on which the TSD will be mounted. A ‘Shaker-Table’ is such a device. Typically they consist of a steel table attached by pin-joints to a series of electronically controlled hydraulic actuators. The TSD is bolted down to the table via lateral, and possibly vertical, load cells which measure the force transmitted to the TSD. Vertical cells are required if it is desirable to know the moment applied to the TSD. The other output of interest from the experiments is the sloshing height, this can be measured by fixing a depth gauge to the TSD tank immersed at the extremity of the sloshing liquid. A schematic of a typical experimental set-up is shown. depth gauge lateral load cell ‘Shaker-Table’ 5.6.5.4.2 Measuring Damping Invariably the purpose of laboratory tests on TSDs is to establish the damping ratio. There are three ways in which this can be attempted: 1. Logarithmic-decrement method 2. Half power-point method 3. Random decrement method 872 Structural Engineering Analysis and Design Second Edition 5.6.5.5 5.6.5.5.1 Miscellaneous Design Information Separator-Plates It will often be the case that several damper tanks are required to achieve the required damper mass. In this case it might prove economic to manufacture one large tank then segment this longitudinally and transversely with separator plates. Longitudinal Separator-Plates In the longitudinal (slosh-wise) direction the plates are installed to prevent excessively large transverse waves due to reflections. The rule of thumb used is to limit the breadth of each individual slosh tank to half its length. As the longitudinal plates will have little or no dynamic head difference across them, the seal surrounding the separator plate is of little importance. Neither, for the same reason, is there a requirement for them to be particularly stiff. Transverse Separator-Plates In contrast, the transverse separator plates have a significant dynamic force across them when the TSD is excited as shown in figure below. For a given water height, translating the plate back and for changes the sloshing frequency of a TSD so transverse plates will also be required when TSDs are being designed for structures whose natural frequency is not accurately known. If there is excessive flexure of the plates during operation then the normal mode of the TSD will be modified slightly and, experiments indicate that, the natural frequency will be reduced. The seal surrounding transverse separator plates has a significant impact on the performance of the damper. head difference 2 1 Seepage under separator-plate At the sloshing extremity shown above, TSD liquid will seep from damper 1 to damper 2 at a maximum rate. Half a cycle later, water will seep in the opposite direction at a maximum rate. The continuous passage of the liquid backand-for under the separator-plate introduces damping into the TSD. The characteristics of the damping introduced are dependent on the size of the gap surrounding the separator-plate. As the gap is reduced, the ‘magnitude’ of the damping will reduce yet the viscous element of damping will increase (due to the fall in the Re number). The effect of the gaps was to introduce a considerable amount of damping at low-excitation levels, in effect ‘linearising’ the damper to some degree. Damping levels at higher excitation levels were found to be closer to predictions, the reason being that the proportion of the damping due to seepage was small compared to the liquid passing the Damping Elements at a higher rate. 5.6.5.5.2 Additional Considerations Add anti-freeze if a TSD is to be used externally. Stagnant pools need to be treated for algae and legionaires’ disease. Seal the tank, evaporation will change the TSDs slosh frequency and affect the performance 873 Structural Engineering Analysis and Design Second Edition 5.6.5.6 Design Procedure for Deep Tank TSDs The following is a suggested possible design process for deep tank TSDs: 1. Establish the level of damping required for desired structural response and convert this to an equivalent peak DAF ( = ½ε). 2. Select a suitable damper to structure modal mass ratio, µ. e.g. using figure below. NB. The DAFs in the figure are for optimum damping and are unlikely to be achievable in practice. structural damping Max DAF at opt. damping Mass ratio (Mdamper /Mstructure ) 1 f structure . 1+ µ 3. Calculate the optimum TSD sloshing frequency using f opt = 4. Choose TSD dimensions such that f 1 = 1.02 f opt using the sloshing frequency formula (The factor of 1.02 accounts for the likely frequency shift due to damping and blockage in the TSD). 5. Calculate M1 (the active sloshing mass of the TSDs) based on the chosen TSD dimensions (assume a breadth of half the length). 6. Calculate the number of dampers required to provide the required mass ratio using N = µM mod al M1 . Do the dampers fit in the space available? 7. Select a ‘K’ (damping per sloshing height) value from table of values presented before and assume εo=0.03. 8. 9. Plot the DAF for the system in a spreadsheet. If the DAF is below the desired level across the required frequency range, start a sensitivity study (try varying f1 , M1 and K). If not, inspect a plot of the damping against frequency, try changing K (within reason) so that the damping is closer to optimum in the region of interest. If this doesn’t work, try a higher mass ratio. 874 Structural Engineering Analysis and Design Second Edition 5.7 GL, ML Active Structural Motion Control – Control System Analysis A control system provides feedback (output) to an input. This is useful to model an Active Mass Damper (AMD). The modelling of a control system involves the definition of an input-output relationship, i.e. a transfer function. This can be defined using the TF bulk data entry. Nonlinearities can be simulated via the NOLINi entries with which nonlinear transient loads are expressed as functions of displacements or velocities. Complex eigenvalue analysis can be used to determine stability when control systems include damping and unsymmetrical matrices. 875 Structural Engineering Analysis and Design Second Edition 5.8 5.8.1 Fibre Reinforced Polymer (FRP) Analysis and Design 17 Introduction A Fibre Reinforced Polymer (FRP) composite laminate is a material composed of plies. Each ply consists of fibres within a polymer matrix with the addition of additives. The fibres impart strength and stiffness to the composite and also act as crack stoppers for good fatigue resistance. The matrix binds the fibres together, transferring loads from fibre to fibre. The matrix also protects the fibres from mechanical abrasion and chemical reactions with the environment. The mechanical properties are predominantly governed by the fibres; fibre type, fibre length, fibre volume fraction and fibre orientation. The chemical properties, behaviour in fire and durability are largely governed by the properties of the matrix polymer. Together, the FRP composite presents a robust material solution with good stiffness/weight and strength/weight ratios, good fatigue and corrosion resistance and favorable cost savings in transportation, assembly and construction due to its relatively light weight despite its unfavorable material cost / weight ratio. 5.8.2 The Reinforcement Fibre Property Glass Carbon Aramid (Kevlar TM) Tensile Strength, σf, ult (MPa) Compressive Strength, σf, ult (MPa) E-Glass: 2500 R-Glass: 3200 HT-Carbon: 3200 HM-Carbon: 2500 2900 E-Glass: Efℓ = 74 Eft = 74 Gf = 30 R-Glass: Efℓ = 86 Eft = Gf = Glass fibre is isotropic. E-Glass: 0.25 R-Glass: 0.2 Low; E-Glass: 2600 R-Glass: 2500 HT-Carbon: Efℓ = 230 Eft = 15 Gf = 50 HM-Carbon: Efℓ = 390 Eft = 6 Gf = 20 Carbon fibre is anisotropic. HT-Carbon: 0.3 HM-Carbon: 0.35 Very Low; HT-Carbon: 1750 HM-Carbon: 1800 Low; 2.5 High; 10.0 – 200.0 High; 20.0 Low; E-Glass: 0.5E-5 R-Glass: 0.3E-5 Very low; HT-Carbon: 0.02E-5 HM-Carbon: 0.08E-5 Low; -0.2E-5 Dependent upon elastic strain energy absorbed; Dependent upon elastic strain energy absorbed; Dependent upon elastic strain energy absorbed; Stiffness (GPa) Poisson’s Ratio, νf Density, ρf (kg/m3) Material Cost 18 ₤ / kg Coefficient of Thermal Expansion, αf (Strain/°C) Impact Resistance (Brittle Failure Toughness) Fatigue Fire Efℓ = 130 Eft = 5.4 Gf = 12 Aramid fibre is anisotropic. 0.4 Very Low; 1450 See Section 5.8.3. Retain strength up till melting point (over 1000 Oxidise in air above 650 °C. Combustible. Limited to 200 °C. Combustible. 17 GAY, Daniel, HOA, Suong, TSAI, Stephen. Composite Materials Design and Application. CRC Press, London, 2003. 18 NB: Cost reductions are however made in erection and transportation due to the lighter weight. 876 Structural Engineering Analysis and Design Second Edition °C). Combustible. Not susceptible. Susceptible only when in contact with aluminium causing a “galvanic phenomenon” which leads to rapid corrosion. Coefficient of Thermal Conductivity at 20°C, λ (W/m°C) Heat Capacity, c (J/kg°C) Low; E-Glass: 1 R-Glass: 1 E-Glass: 800 R-Glass: 800 Very high; HT-Carbon: 200 HM-Carbon: 200 HT-Carbon: 800 HM-Carbon: 800 Electrical Conductivity Non-conducting. Conducting. Chemical Resistance Attacked by alkalis (pH greater than 11) but not by acids. Good. UV Resistance Good. Good. Sustainability Non-toxic and inert. Does not contaminate groundwater. Non-toxic and inert. Does not contaminate groundwater. Corrosion Resistance Not susceptible. Creep Transparency to Radio Frequency Electromagnetic Considerations 877 Very low; 0.03 1400 Non-conducting. Aramids absorb much more water than either glass or carbon causing problems with the resin/fibre interface. Changes colour and the strength reduce. However, when embedded in resin, overall mechanical properties little affected. Non-toxic and inert. Does not contaminate groundwater. Structural Engineering Analysis and Design Second Edition 5.8.3 The Polymer (Resin) Matrix There are two types of polymer; thermosets and thermoplastics. Once cured (hardened) by a chemical reaction, a thermosetting polymer will not melt or soften when subsequently heated. A thermoplastic polymer softens when heated and hardens upon cooling. Common thermoset polymers are polyester, epoxy and phenolic. Property Polyester Epoxy Phenolic 80 130 70 Stiffness (GPa) Em: 4.5 Gm: 1.4 Polyester is isotropic. Em: 4.5 Gm: 1.6 Epoxy is isotropic. Em: 3.0 Gm: 1.1 Phenolic is isotropic. Poisson’s Ratio, νm 0.4 0.4 0.4 Density, ρm (kg/m3) 1200 1200 1300 2.5 5.0 – 10.0 10.0 High; 8E-5 High; 11E-5 Low; 1E-5 Tensile Strength, σm, ult (MPa) Compressive Strength, σm, ult (MPa) Material Cost ₤ / kg Coefficient of Thermal Expansion, αm (Strain/°C) Impact Resistance (Brittle Failure Toughness) Fatigue Fire Fatigue resistance of FRP composites is generally better than that of metals as the fibres act as crack stoppers - up to 1000000 cycles no fatigue limit. Unlike metals, fatigue failure is gradual as the matrix cracks and fibres debond. Generally, nonpropagating stress range estimates for composites can be as high as 90% of static strength (cf. that for steel and titanium being 50% and aluminium 35%). Although the fibres are not flammable, the polymer matrix is inherently flammable. Although thermoset polymers do not melt when heated, they do soften (Young’s Modulus decreases) above the glass transition temperature Tg, typically 60 – 70 °C. This greatly influences the maximum service temperature of a FRP composite and its structural performance in a fire. The temperature at which a FRP composite softens is called the Heat Distortion Temperature (HDT) and is related to Tg. Corrosion Resistance Creep All polymers used in FRP composites display viscoelastic or time (and temperature) dependent properties. Materials with a high glass transition temperature (Tg) have higher creep resistance. Creep is of primary significance for structures under a sustained load. Creep in FRP composites is primarily a matrix deformation. A FRP composite with fibres aligned in the direction of the applied stress, creep is unlikely to be a significant problem, while loading off axis to the fibre direction may result in excessive deflection. The design methodology should be based on limiting the internal strains in the matrix. Axial strain levels should be less than 0.2% strain. Creep curves are available for estimating creep modulus (long term modulus). Coefficient of Thermal Conductivity at 20°C, λ Low; 0.2 Low; 0.2 878 Low; 0.3 Structural Engineering Analysis and Design Second Edition (W/m°C) Heat Capacity, c (J/kg°C) 1400 1000 1000 Chemical Resistance Resistant to grease, oils, paints, solvents, petroleum. Polyester resins attack polystyrene foam in sandwich structures. Resistant to grease, oils, paints, solvents, petroleum. Epoxy resins can absorb water by diffusion up to 6% of mass. Paint thinners attach epoxy resins. Resistant to grease, oils, paints, solvents, petroleum. UV Resistance Good. Maintains appearance > 20 years. Used as protective gel coat on composites with a more UV sensitive polymer. Appearance changes long before significant mechanical property degradation. Electrical Conductivity Sustainability Transparency to Radio Frequency Electromagnetic Considerations An application where it has been particularly useful to use FRP composites is where concrete members require non-ferrous reinforcement due to electromagnetic considerations e.g. MRI scanner rooms; airport radio and compass calibration pads; high voltage electrical transformer vaults; concrete near high voltage cables and substations. 879 Structural Engineering Analysis and Design Second Edition 5.8.4 The Additives Property Remark UV Resistance To counteract UV effects on appearance and the degradation of mechanical properties, additives can be blended with the polymer during processing. Photo stabilizing additives protect the polymer chains by reacting preferentially with UV light - UV absorbers. Pigments can also protect the polymer by reflecting the UV radiation. Metallic pigments can be used as effective reflectors. Zinc oxide (ZnO) is another effective reflector. However, the most effective reflector is carbon black. It is often used to enhance the lifespan of polymers exposed outdoors. Colors that can be particularly prone to fade include reds, yellows and pastel colors. 880 Structural Engineering Analysis and Design Second Edition 5.8.5 The Composite Laminate Forming Processes Forming Process Description Contact Molding (Hand Lay Up) Compression Molding Molding impregnation of fibres into resin placing mixture on tool compaction polymerization demolding finishing Sheet Forming Profile Forming (Pultrusion) Stamp Forming Three Dimensional Assembly Cutting Vacuum Assisted Resin Transfer Molding VARTM (a.k.a. Depression Molding or Bag Molding) Open molding since there is only one mold. Reinforcement is mats or fabrics. Compaction is done using a roller to squeeze out air pockets. Labour intensive and high quality workmanship required. Closed molding as the countermold will close the mold to apply pressure after impregnated reinforcement (fabrics or unidimensionals) placed on mold. Vacuum is applied under a soft plastic sheet on the open mold and piece is compacted under atmospheric pressure to elimitate air bubbles. Resin is injected into the preformed reinforcement (unidimensionals, fabrics, mats) placed between the mold and countermold. Premixed (a.k.a. Bulk Moulding Compound B.M.C., i.e. Injection of Premixed mixture of cut short fibres in a resin matrix) is fed into Molding mold and countermold in a highly automated fashion. Molding by foam injection allows the processing of polyurethane foam reinforced with glass fibres in mold Foam Injection Molding and countermold. Allows for the fabrication of tubes using short fibres. Centrifugal Molding Filament winding is used to form tubes with continuous fibres wound helically within the component. The fibres are coated with polymer resin and wound around a Filament Winding mandrel to create the desired shape. The winding angle may be varied to orientate the fibres to give the desired properties in different directions. Allows the production of plane or corrugated sheets. Pultrusion involves pulling reinforcement fibres (unidimensionals, fabrics or mats) coated in a polymer resin through a die. Only applicable to thermoplastic composites. Preformed plates are heated, stamped and then cooled. Resin Transfer Molding RTM Woven tows along several directions in space assembled before impregnation using liquid or gas. A programmed cutting machine can cut components into shapes required by the design. 881 Structural Engineering Analysis and Design Second Edition 5.8.6 Modelling and Analyzing MSC.NASTRAN 5.8.6.1 Fibre Reinforced Polymer (FRP) Composite Laminates in The Ply The reinforcement fibres are manufactured to be as thin in diameter (d) as possible because their rupture strength decreases as their diameter increases. The minimum effective fibre length (critical fibre length, lc) is dependent on the fibre diameter (d) and its ultimate tensile strength, σf, ult and on the fibre-matrix bond strength (or the shear strength of the matrix) τc according (simplistically) to lc = σf, ult d / τc For a number of glass and carbon fibre-matrix combinations, this critical length is on the order of 1 mm, which ranges between 20 and 150 times the fibre diameter. Fibres for which l >> lc (normally l > 15lc) are termed continuous; discontinuous or short fibres have lengths shorter than this. For discontinuous fibres of lengths significantly less than lc, the matrix deforms around the fibre such that there is virtually no stress transfer and little reinforcement by the fibre. The forms of the reinforcement fibres are i. Unidimensional (continuous fibres) ii. Bidimensional woven fabric (continuous fibres) iii. Bidimensional mat (short or continuous fibres) iv. Multidimensional fabric (continuous fibres) 5.8.6.1.1 Mechanical Properties of the Unidimensional Ply Two dimensional anisotropic materials (MAT2) can be fully defined from 7 independent constants, Ex, Ey, νyx, νxy, Gxy, Gxz, Gyz.  Ex  1 − ν xy ν yx σx      ν xy E y σ y  =  τ  1 − ν xy ν yx  xy   0   ν yx E x 1 − ν xy ν yx Ey 1 − ν xy ν yx 0  0    ε x  α x       0   ε y  − (T − Tref )α y    γ   0    G xy   xy    τ xz  G xz  = τ yz   0 0  γ xz    G yz  γ yz  Two dimensional orthotropic materials (MAT8) can be fully defined from 6 independent constants, 3 from Ex, Ey, νyx and νxy due to the symmetry relation νxyEy = νyxEx and also Gxy, Gxz, Gyz.  Ex  1 − ν xy ν yx σx   ν xy E y    σ y  =  τ  1 − ν xy ν yx  xy   0   ν yx E x 1 − ν xy ν yx Ey 1 − ν xy ν yx 0  0    ε x  α x       0   ε y  − (T − Tref )α y    γ   0    G xy   xy    τ xz  G xz  = τ yz   0 0  γ xz    G yz  γ yz  Two dimensional (plane stress) isotropic material (MAT1) can be fully defined from 2 independent constants from E, G and ν as G = E / [2(1+ν)]. 882 Structural Engineering Analysis and Design Second Edition  E  σ x  1 − ν 2    νE σ y  = 2 τ   1 − ν  xy   0   νE 1− ν2 νE 1− ν2 0  0  α    ε x    0   ε y  − (T − Tref )α      0    G  γ xy    τ xz  G 0  γ xz   =   τ yz   0 G  γ yz  A fundamental physical difference in the deformation between an isotropic and an orthotropic material shall be mentioned. If an isotropic material is stressed, the deformation of the element will be ellipsoidal with the axes of the ellipsoid coinciding with the principal stress axes. However, if an orthotropic material is stressed, the deformation of the element will be ellipsoidal with the axes of the ellipsoid not coinciding with the principal stress axes. The mechanical properties of a ply are defined on the MAT8 card. Note that x denotes the longitudinal direction of the ply, y the transverse in plane direction of the ply and z the transverse out of plane direction of the ply; f denotes fibre and m the resin matrix; fℓ the longitudinal direction of the fibre and ft the transverse direction of the fibre. Property of Ply Expression The longitudinal modulus, Ex (or E1) (Assumes straight and unidirectional fibre orientation and that the material is bimodulus, i.e. same stiffness in tension and compression) Ex = EmVm + EfℓVf = Em(1–Vf) + EfℓVf The in-plane transverse modulus, Ey (or E2) The in-plane Poisson’s ratio, νxy (or NU12)     V V 1 1  or = m + f Ey = Em  E y E m E ft  (1 − V ) + E m V  f f   E ft   νxy = νmVm + νfVf = νm(1–Vf) + νfVf     1  G xy = G m  The in-plane shear modulus, Gxy (or G12) Gm    (1 − Vf ) + G Vf  f   If test data are not available, the value of G12 may be The out-of-plane shear modulus, Gxz (or G1Z) used for G1Z and G2Z. If zero then no shear flexibility or shear deformations, i.e. infinite shear stiffness. If test data are not available, the value of G12 may be The out-of-plane shear modulus, Gyz (or G2Z) used for G1Z and G2Z. If zero then no shear flexibility or shear deformations, i.e. infinite shear stiffness. 1 The in-plane modulus along any direction, Eθ Eθ = 4 4  1 ν xy  cos θ sin θ (Note the rapid decrease in modulus in directions  + + 2 cos 2 θ sin 2 θ −   away from the longitudinal fibre) Ex Ey  2G xy E y  883 Structural Engineering Analysis and Design Second Edition where θ = anticlockwise angle from x Mass density, ρ (or RHO) ρ = ρmVm + ρfVf = ρm(1–Vf) + ρfVf The longitudinal coefficient of thermal expansion, α = α f E fλ Vf + α m E m Vm x αx (or A1) E fλ Vf + E m Vm (ν f E m − ν m E fλ ) (α f − α m ) The transverse coefficient of thermal expansion, αy α y = α m Vm + α f Vf + E m E fλ + (or A2) Vf Vm Vf ρ f Mf = Fibre mass fraction, Mf Vf ρ f + Vm ρ m Mm =1− Mf =1− Resin matrix mass fraction, Mm Vf ρ f Vf ρ f + Vm ρ m The fibre volume fraction, Vf depends largely upon the manufacturing process used. Molding Process Fibre Volume Fraction, Vf Contact Molding 30% Compression Molding 40% Filament Winding 60% − 85% Vacuum Molding 50% − 80% Conversely, if the fibre mass fraction Mf is known, the volume fractions can be derived as follows. Property of Ply Expression Fibre volume fraction, Vf Vf = Resin matrix volume fraction, Vm Vm = 1 − Vf = M f / ρf M f / ρf + M m / ρm M f / ρf M f / ρf + M m / ρm The thickness of the plies must be defined on the PCOMP card (for each individual PSHELL card) as Ti. The thickness is obtained as follows. 1 m 1  1 − M f    Ti = of or Ti = m of  + Vf ρ f  ρ f ρ m  M f  where mof is the mass of fibre per m2 of area. 5.8.6.1.2 Mechanical Properties of the Bidimensional Woven Fabric Ply The fabrics are made of fibres oriented along two perpendicular directions, one called the warp and the other called the fill direction. The fibres are woven together, which means that the fill yarns pass over and under the warp yarns, following a fixed pattern. Each fabric layer is considered to be a single anisotropic layer of thickness Ti with approximate mechanical properties as follows. Define n1 k= n1 + n 2 where n1 is the number of warps yarns per metre and n2 is the number of fill yarns per metre. Then Exfabric ≈ kEx + (1–k)Ey Eyfabric ≈ (1–k)Ex + kEy 884 Structural Engineering Analysis and Design Second Edition Gxyfabric ≈ Gxy ν xyfabric ≈ ν xy k + (1 − k ) Ex Ey where Ex, Ey, Gxy and νxy are values obtained by considering the woven fabric ply to be a unidirectional ply, i.e. with both the warp and fill yarns to be in the same direction such that the total volume fraction, Vf would be the same as that of one unidirectional ply. Note that the stiffness of a woven fabric will be less than two equivalent (with the two unidirectional plies having the same fibre volume fraction as the one woven fabric ply) unidirectional plies orthogonal to one another because of the curvature of the woven fibres over and under the orthogonal fibres. The thickness of the anisotropic ply would be Ti as with the unidirectional ply. 5.8.6.1.3 Mechanical Properties of the Bidimensional Mat Ply Mats are made up of short cut fibres or continuous fibres such that they are isotropic within their plane. Hence their properties can be approximated by just two constants (and hence using MAT1) approximately as 3 5 E mat ≈ E x + E y 8 8 E mat G mat ≈ 2(1 + ν mat ) ν mat ≈ 0.3 where Ex and Ey are the elastic moduli along the longitudinal and transverse directions of a unidirectional ply with the same volume fraction Vf. The thickness of the mat ply would be Ti as with the unidirectional ply. 5.8.6.1.4 Mechanical Properties of the Multidimensional Fabric Ply Multidimensional fabric plies has the reinforcement assembled according to pre-established directions. The ply is isotropic within its plane. 885 Structural Engineering Analysis and Design Second Edition 5.8.6.2 The Composite Laminate, Sandwich Structures and Structural Members with Attached Laminates There are three types of laminated construction. These include the all laminated construction consisting of relatively high stiffness and strength layers, the sandwich structure lamination consisting of at least two high stiffness and strength outer layers connected by a core, and a third type consisting of a structural member that is reinforced on the tensile or compression or both sides of a flexural beam. 5.8.6.2.1 Mechanical Properties of the Composite Laminate A composite laminate is comprised of a number of plies. These can be defined using the PCOMP entry that refers to the material cards of the individual plies MIDi, their thickness Ti and the orientation of the ply longitudinal axis from the MCID by THETAi. Plies are always defined bottom up (Z0 = −0.5 x total element thickness ∑Ti). There is a genuine need for a midplane symmetry (ensured by specifying LAM = “SYM”) because during the cooling process of manufacture, the plies have the tendency to contract differently depending on their orientations. With symmetry of the midplane, nonuniform contraction is avoided. [ ] [ ] Typical laminate lay-ups of unidirectional plies are [90/02/−45/45]S and 0 / 45 / − 45 / 90 S . Note that these are defined bottom up. The S-subscript indicates a set of symmetric plies. The 2-subscript indicates two plies. The hyphen above the number indicates that it is the midplane ply. The 0 / 45 / − 45 / 90 S lay-up is really the technological minimum with the minimum thickness of the laminate being around 1mm. The plies should be orientated such that there are fibres orientated in both the maximum and minimum principal stress directions. There should also be no more than 4 consecutive plies along the same direction. The plies should be progressively terminated to obtain a gradual change of thickness (maximum 2 plies for each 6mm interval). Laminate lay-up which are symmetric can also be made up of fabrics, which can be thought of as a pair of orthogonal plies and also of mats, which are isotropic in-plane. 5.8.6.2.2 Mechanical Properties of Sandwich Structures Sandwich structures are made up of two facings sandwiching a light flexible core, hence again definable with a PCOMP entry. The facing can be a composite laminate of many anisotropic MAT8 plies or simply a layer of isotropic MAT1 material such as aluminium. The core can be deemed as just another layer within PCOMP with a relatively much greater thickness. A significant benefit of sandwich structures is the fact that they are extremely light whilst having a high flexural rigidity due to the separation of the surface skins. The mass per unit area of the dome of the Saint Peter’s Basilica in Rome (45m diameter) is 2600 kg/m2 whereas the same dome made of steel/polyurethane foam sandwich (Hanover) is only 33 kg/m2. Very approximate stress formulae in a 3 layer (core T2 sandwiched by 2 facings of thickness T1 and T3) sandwich structure are as follows. These are useful verifications of computer outputs. 886 Structural Engineering Analysis and Design Second Edition M (per unit metre) assuming all bending is resisted by the facings T2 + 1 (T1 + T3 ) (1m width ) 2 V (per unit metre) Shear stress in foam τ = assuming all the vertical shear is resisted by the core T2 (1m width ) Bending stress in facings σ = ( ) The approximate verification of displacements requires the estimation of the stiffness of the sandwich structure. Also, both bending and shear deformations may be significant, hence both bending and shear stiffnesses must be approximated as follows. Note that T2 is the thickness of the core and Tfacings is the thickness of the facings, i.e. T1 or T3. ( width . Tfacings . T2 + Tfacings width . skin thickness . (average panel depth )2 = E facings 2 2 GA s = G core T2 + 2Tfacngs . width EI = E facings ( ) 2 ) Sandwich structures are susceptible to global buckling according to Euler (including shear deformations) as π 2 EI Fcr = K EI L2 + π 2 K GA s where K = 1 for simply supported, K = 4 for fixed ended, K = 2.04 for fixed-pinned and K = 0.25 for cantilever. Sandwich structures are particularly susceptible to local buckling of the facings. The critical compression stress is 1/ 3 3 2 σ cr = E facings E core 2 2 1/ 3 12(3 − ν core ) (1 + ν core ) [ ] ( ) The axial critical force in a beam for local buckling of the facings is approximately  E Tfacings Fcr = 1.64Tfacings .width.E facings  core  E facings T2  5.8.6.2.3     1/ 2 Mechanical Properties of Structural Members with Attached Laminates This is utilized most often in construction and infrastructure applications. PCOMP can be used to define the attached composite laminates on the flanges of the structural members, but of course not the structural members themselves because the orientation of the web will be orthogonal to the orientation of the flange. Hence define explicit PSHELL entries for the structural members. 887 Structural Engineering Analysis and Design Second Edition 5.8.6.3 Failure Mode and Failure Criteria of the Composite Laminate The failure mode of a ply is brittle rather than ductile with no significant yielding until failure at the ultimate tensile strength. The ply remains elastic until the ultimate limit strength. In light of this it has been assumed that only elastic methods may be used, with no redistribution. If the loading is tensile along the direction of the fibres, it is assumed that the fibres break before the matrix. The compressive strength along the direction of the fibres will be smaller than the tensile strength along the same direction due to the micro buckling phenomenon of the fibres in the matrix. To define a failure criteria a failure theory must be specified on the FT field of the PCOMP entry from either “HILL” for Hill-Tsai, “HOFF” for Hoffman, “TSAI” for Tsai-Wu or “STRN” for maximum strain theory. The allowable inter-laminar shear stress SB needs also to be provided in the PCOMP card in case of inter-laminar failure. Then on the MAT8 cards, the allowable stress or strain in tension and compression in longitudinal direction Xt, Xc, in the transverse direction Yt, Yc and the allowable stress or strain for in-place shear, S is required. Hill-Tsai is really for orthotropic materials with equal strengths in tension and compression. The Hoffmann and Tsai-Wu theory are for orthotropic materials with general state of plane stress with unequal strengths in tension and compression. Note that the Hoffmann theory takes into account the difference in tensile and compressive allowable stresses by using linear terms in its equation. The Tsai-Wu however is complicated by the need to satisfy a stability criterion with an experimentally (biaxial loading) derived parameter F12 defined on the MAT8 card. Narayanaswami and Adelman have thus suggested that F12 be set to zero and the use of Hoffman's Theory or the Tsai-Wu theory with F12 = 0 are preferred alternatives. STRN on the MAT8 with a value of “1.0” is additionally required for the maximum strain theory to indicate that Xt, Xc, Yt, Yc and S are strain allowables, instead of stress allowables for the other criteria. 888 Structural Engineering Analysis and Design Second Edition The maximum strain criteria failure index is defined as follows STRN can also be left blank (as done for the other criteria) even for the maximum strain theory to allow stress allowables in which case the maximum strain criteria becomes the maximum stress criteria. For this case the failure indices are calculated using The failure index of the bonding material will be calculated as the maximum interlaminar shear stress divided by the allowable bonding stress. Classical lamination theory, which utilizes the plane stress assumption, does not account for interlaminar stresses. As a result, this theory cannot be used to predict the magnitude of these stresses. High values of these interlaminar stresses can lead to failures that are unique to composite materials. An approximate technique is used to calculate the interlaminar shear stresses. The basic assumption in this approximate technique is that the x- and y-components of stress are decoupled from one another. The interlaminar shear strains are calculated by The Hill-Tsai failure criterion is defined as follows for each and every ply.  σ α=  x σ  x , ult 2  σ   + y   σ y , ult   2   τ σ σ  − x y +  xy 2  σ x , ult  τ xy, ult  2   < 1.0 for no ply rupture    E  where σ x, ult = σ f, ult Vf + (1 − Vf ) m  ≈ σ f, ult Vf E fλ   These correspond to the entries on the MAT8 cards, the allowable stress in tension and compression in longitudinal direction Xt (σx, ult), Xc (σx, ult), in the transverse direction Yt (σy, ult), Yc (σy, ult) and the allowable stress for in-place shear, S (τxy, ult). If α > 1, then rupture occurs in the ply considered, generally due to the rupture of the resin. The rupture resistance does not have the same value in tension and compression, hence it is useful to place in the denominators of the Hill-Tsai expression the rupture resistance values corresponding to the mode of loading (i.e. whether tension or compression) that appear in the numerator. This is done automatically in NASTRAN as follows. 889 Structural Engineering Analysis and Design Second Edition 5.8.6.4 MSC.NASTRAN Finite Element Modelling of Composite Laminate Summary Classical lamination theory is employed, hence incorporating the following assumptions: i. The laminate consists of perfectly bonded laminae or ply. ii. The bonds are infinitesimally thin and nonshear-deformable; i.e., displacements are continuous across laminae (or ply) boundaries so that no lamina can slip relative to another. iii. Each of the ply is in a state of plane stress. The PCOMP property card is used for modelling a composite material consisting of layers. This information is used internally within NASTRAN to compute equivalent PSHELL cards. The information on the PCOMP card includes the thickness, orientation and material identification of each layer. This information is used internally within NASTRAN to compute equivalent PSHELL cards. Special layer-by-layer output is provided when the PCOMP option is used. We have said that for shells, the element definition and element stress recovery are performed in the element coordinate system by default (but defined by MCID entry on element connection card; 0 for basic projected, > 0 for user projected, < blank > for element coordinate system, > 0.0 and < 360.0 for angled from side n1-n2 of element). (Note that for beams, the element definition and element stress recovery are performed in the element coordinate system. For solid elements, the element definition and element stress recovery are performed in the basic coordinate system by default (but defined on CORDM field of PSOLID; 0 for basic, > 0 for user-defined, -1 for element coordinate system)). In the case of the PCOMP entry, the element coordinate system requires further subdivision as there are many plies. Hence the THETAi field of the PCOMP entry specifies the angle from the coordinate system defined by MCID on the element connection card for the longitudinal axis of each ply i. To define laminates with PCOMP and numerous orthotropic MAT8 cards, the following procedure is undertaken. I. Define a common material coordinate system MCID for the CQUAD4 elements. This would refer to either the basic coordinate system (by specifying “0”) or a user-defined coordinate system (by specifying a CORDij ID). In the usual case of uniform isotropic shells, MCID can be left defaulted to the individual element coordinate system (by specifying < blank >), random as they may be, because due to the nature of the elements being uniform and isotropic, the geometric definition will be the exact, and the correct consistent stress recovery will be obtained so long as the stresses are rotated onto the global axes system by the post-processor (of course though the Z-normal must still be ensured to be coherent amongst adjacent elements for correct stress recovery of top and bottom surfaces). But in the case of the orthotropic shell, the geometric definition requires a coordinate system. It is best to define a single user defined coordinate system for all the elements on their MCID field, noting that the element coordinate system will then be the projection of the defined system onto the element plane. The thickness T1 to T4 should not be specified because in accordance with normal practice of defining isotropic materials, thickness is specified in the property card. II. Define a PCOMP card that refers to the material cards of the individual plies MIDi, their thickness Ti and the orientation of the ply longitudinal axis from the MCID, THETAi. Plies are always defined bottom up (Z0 = −0.5 x total element thickness ∑Ti). SOUTi field requests by “YES” or “NO” stress output for the individual plies provided that the ELSTRESS case control command is specified. The LAM field specifies the laminate option from < blank > for explicitly specifying all plies, the recommended “SYM” for specifying half the symmetrical plies from bottom side (with centerline ply of half thickness if odd-number of plies within laminate), “MEM” for specifying all the plies but with membrane stiffness only (MID1 on derived PSHELL) and “BEND” for specifying all the plies but with bending stiffness only (MID2 on derived PSHELL). A failure theory FT can be specified from “HILL” for Hill-Tsai, “HOFF” for Hoffman, “TSAI” for Tsai-Wu or “STRN” for maximum strain theory. The allowable inter-laminar shear stress SB needs to be provided. 890 Structural Engineering Analysis and Design Second Edition III. Define an orthotropic MAT8 card (although a MAT1 card could be used for a mat ply) for each individual ply. For each ply, need to define E1, E2, Poisson’s ratio NU12, in-plane shear modulus G12, transverse shear modulus for shear in 1-Z plane G1Z, transverse shear modulus for shear in 2-Z plane G2Z (if G1Z and G2Z zero, then no shear flexibility or shear deformations, i.e. infinite shear stiffness) and density RHO. Define the thermal expansion coefficients A1 and A2 if necessary. If the failure criterion is requested in PCOMP (in field FT), then the allowable stress or strain in tension and compression in longitudinal direction Xt, Xc, in the transverse direction Yt, Yc and the allowable stress or strain for in-place shear, S is required. F12 is additionally required for Tsai-Wu failure criterion. STRN with a value of “1.0” is additionally required for the maximum strain theory to indicate that Xt, Xc, Yt, Yc and S are strain allowables instead of stress allowables. STRN can also be left blank (as done for the other criteria) even for the maximum strain theory to allow stress allowables in which case the maximum strain criteria becomes the maximum stress criteria. Safety factors vary considerably depending upon laminate design, constituent materials, manufacturing method, service conditions, etc. However, as a rule of thumb, a conservative value of 3 can be used for the material factor. The following are the MSC.NASTRAN recovered outputs:i. stress (ELSTRESS) and strain (ELSTRAIN) for the equivalent laminate shell ii. force resultants (ELFORCE) iii. stresses and strains in the individual plies and the shear stress in the bonding material iv. a failure index table (if Xt, Xc, Yt, Yc and S specified on MAT8 and FT and SB specified on PCOMP) The failure index for an element is the largest value of the failure indices for all plies of the element. 891 Structural Engineering Analysis and Design Second Edition 6 FINITE ELEMENT MODELLING TECHNIQUES AND MSC.NASTRAN CARDS COMMON TO ALL ANALYSES NASTRAN was originally developed by NASA for the space program at the end of the 1960’ s. It is an extremely sophisticated and complicated general-purpose finite element analysis program. 6.1 Input Deck .dat Format A NASTRAN input file is a .dat file. There are 3 input formats. In the small-field fixed format, each card of 10 fields has fields of 8 characters each. In the large-field fixed format, each card of 6 fields has fields of 16 characters except the first and the last which is still 8 characters. The large-field format is denoted by having an asterisk (*) immediately following the card name in the first field. The fields in the free-field format are separated by commas and their accuracy is similar to the small-field fixed format. Hence, real numbers greater than 8 characters will lose precision when in the free-field format. The Bulk Data Section can utilize any format, whilst the other sections utilize the free-field format. $ in the very first column denotes a comment line. The entries for the fixed format cards may be anywhere within the Field except for entries in Field 1 and 10 which must be left-justified. The first field gives the card name whilst the last field is reserved as a continuation field. It is important to ensure that the right data type (between Integer, Real or Character) is entered; Integers cannot contain a decimal point, Reals must contain a decimal point and Characters can be alphanumeric although must start with an alpha character and must be equal or less than 8 characters. NASTRAN will not proceed with the analysis if the wrong type of data is detected. Continuation cards are best automatically generated by leaving the last field of the initial card and first field of the next card blank. Automatic continuation cards are not generated for the large-field format, hence must be entered manually. Never leave blank lines as they will just be ignored. Hence, if a deck consists of 3 cards and the second line is left blank, the third card will be taken as the second card. The format of the input deck is shown as follows. All elements in the model should have unique element IDs, even elements of different types. The formulation of the element stiffness matrix is independent of how the element grid points are numbered. However, each element will have an element coordinate system which is defined by how the element grid points are numbered. $ EXECUTIVE CONTROL SECTION ID <8 character string>, TIME , CEND $ CASE CONTROL SECTION $ TITLE = < TITLE OF JOB > SUBTITLE = < SUBTITLE OF JOB > LABEL = < LABEL OF JOB > $ ……… $ $ BULK DATA BEGIN BULK $ ……… $ ENDDATA The .f06 file should be checked for USER FATAL error messages, which crashes the analysis and USER WARNING error messages, which affects accuracy but does not crash the analysis. Also USER INFORMATION messages 892 Structural Engineering Analysis and Design Second Edition should be read. The .f04 file contains all data associated with the execution of the solution sequence along with system parameters such as memory and disk usage. It also lists the allocation of files. Generally the most useful information in the .f04 file is the total scratch database size. This should be recorded and used when subsequently running models of a similar size. Search for the string MAXIMUM DISK USAGE. The .acct file is the job accounting file and contains useful data such as elapsed time, cpu time, maximum memory used etc. This data can be useful in planning other, similar jobs in future. If the job is very large then the I/O performance can be assessed by looking at the ratio of cpu to elapsed time. Displacement vector sets in NASTRAN define the equations of motion and are partitioned in the following ways. (i) g-set is the unconstrained set of structural equations (ii) the g-set is partitioned into the m-set pertaining to the dependent set of DOFs and the n-set pertaining to the independent set of DOFs g-set − m-set = n-set (iii) the n-set is then partitioned into s-set pertaining to the constrained DOFs and the f-set pertaining to the unconstrained DOFs n-set − s-set = f-set (iv) the f-set is partitioned into the o-set pertaining to the DOFs eliminated by static condensation and the a-set pertaining to the a-set (analysis set) pertaining to the DOFs not eliminated by static condensation f-set − o-set = a-set (v) the a-set is partitioned into the q-set pertaining to the generalized coordinates in Generalized Dynamic Reduction (GDR) or component mode synthesis and the t-set pertaining to the physical DOFs a-set − q-set = t-set (vi) the t-set is partitioned into the r-set pertaining to the SUPORT DOFs and the l-set pertaining to DOFs not placed in a SUPORT entry t-set − r-set = l-set (vii) the l-set is partitioned into the c-set pertaining to the free boundary set for component mode synthesis or dynamic reduction and the b-set pertaining to the coordinates fixed for component mode analysis or dynamic reduction l-set − c-set = b-set Some additional sets include (i) the e-set representing the extra dynamic DOFs from control systems and other nonstructural physical variables (ii) the sa-set representing the permanently constrained aerodynamic points in aeroelastic analysis (iii) the k-set representing the aerodynamic points in aerodynamic analysis Hence, some combined sets include (i) the d-set which is a combination of the a-set and the e-set a-set + e-set = d-set (ii) the fe-set which is a combination of the f-set and the e-set f-set + e-set = fe-set (iii) the ne-set which is a combination of the n-set and the e-set n-set + e-set = ne-set (iv) the p-set which is a combination of the g-set and the e-set g-set + e-set = p-set (v) the ps-set which is a combination of the p-set and the sa-set p-set + sa-set = ps-set (vi) the pa-set which is a combination of the ps-set and the k-set ps-set + k-set = pa-set The output can be printed (into ASCII .f06), punched (into ASCII .pch) or plotted (into binary .op2). The ASCII output can also be outputted in a XY format for simplicity if desired. To print into the ASCII .f06, punch into the ASCII .pch or plot into the binary .op2, the relevant output commands are specified, depicted for example as follows. 893 Structural Engineering Analysis and Design Second Edition $ CASE CONTROL SECTION DISPLACEMENT (, , ) = ALL/ Further, to request binary plotted output, the format of the .op2 file must be specified. PARAM, POST, -2 The output coordinate system can be in the basic coordinate system or the global coordinate system. PARAM, OUGCORD, BASIC To request simple XY output to be either printed or punched, the following is specified. Note that within the XYPLOT section, the format of the output (i.e. whether Real and Imaginary or Magnitude and Phase) where relevant is determined by that which is specified in the general output request, here DISP. The output set of the general output request DISP does not need to reference the grids whose component outputs are being plotted out in the XYPLOT, thus only the format is taken. Note however that the general output request must specify PLOT. If only the XYPLOT is desired and not the binary .op2 file, the PARAM, POST should just not be specified. Failure to specify the general output request would result in the default format for the XYPLOT. Also note that the XYPLOT section must be the very last request in the Case Control Section. $ CASE CONTROL SECTION DISPLACEMENT (,) = ALL/ $ XY plot output OUTPUT(XYPLOT) XYPRINT DISP RESPONSE /() XYPUNCH DISP RESPONSE /() A useful output option is stress sorting. Stress sorting is useful to limit the amount of output to say stresses in elements that only exceed a certain stress criteria. Stress sorting can be performed in MSC.NASTRAN for SOL 101, SOL 109 and SOL 112 using a few parameters. To enable stress sorting PARAM, S1, 1 $ Enables stress sorting To limit the printed and plotted stresses to include only those in the highest 400 say elements PARAM, NUMOUT, 400 say If NUMOUT, 0 is specified, then stresses in all element greater than BIGER say 200000 Pa is printed and plotted. PARAM, BIGER, 200000 say PARAM, SRTOPT controls the sorting method based on maximum or minimum magnitude or maximum or minimum algebraic value. The default is to sort based on maximum magnitude. PARAM, SRTELTYP specifies the element type, default being all elements. Stress sorting is based upon different stress parameters for different element types. For instance the default stress quantity for CQUAD4 is von Mises on the Z2 surface. The default stress parameters may be changed using the DTI, INDTA bulk data entry. 894 Structural Engineering Analysis and Design Second Edition 6.2 Grid Cards $ BULK DATA GRID ID CP X1 X2 X3 CD PS SEID CP is the spatial coordinate system (basic coordinate system (0) or a local user-defined coordinate system) CD is the DOF, output, constraints and solution vector coordinate system (basic coordinate system (0) or a local user-defined coordinate system) There are three coordinate systems in NASTRAN, namely: (a) the basic coordinate system, i.e. an implicitly defined rectangular default coordinate system (b) local user–defined coordinate systems which can be rectangular, cylindrical or spherical (c) element coordinate systems The global coordinate system in NASTRAN is defined as all the coordinate systems defined in the CD field. Hence the global coordinate system, which is the system in which the structural matrices are assembled, is really a collection of basic and local coordinate systems. Classical finite element books state that element stiffness matrices are generated in the element coordinate system and then transformed into a unique coordinate system, which they call the global coordinate system, in NASTRAN the basic coordinate system. NASTRAN on the other hand, generates the element stiffness matrices in the element coordinate system, then instead of transforming that into the unique basic coordinate system, these matrices are transformed into the coordinate system specified on the CD field for the grid points where the element is attached, hence called the global coordinate system. Hence if the CD field of all the grid entries are 0 or left blank, then the global coordinate system will be equal to the basic coordinate system. The user defined local coordinate systems include: Rectangular CORD1R defined by 3 grids Cylindrical CORD1C defined by 3 grids Spherical CORD1S defined by 3 grids Rectangular CORD2R defined by 3 points defined by an independent coordinate system Cylindrical CORD2C defined by 3 points defined by an independent coordinate system Spherical CORD2S defined by 3 points defined by an independent coordinate system If the location of the grids changes then obviously the definitions of the CORD1R, CORD1C and CORD1S local systems also change. If a grid point is not attached to the structure in any way, there will be not stiffness contribution to it. It may be that it is required to define a local coordinate system or an element orientation vector. In this case, the grid point should be fully constrained, either manually with SPC cards or automatically with AUTOSPC. 895 Structural Engineering Analysis and Design Second Edition 6.3 6.3.1 Finite Element Modelling Techniques Nature of the Finite Element Method Shape functions must for convergence in the limit: (i) (ii) permit rigid body motion of the element i.e. zero strain or stress condition (satisfied by having a constant term in the interpolation function) have its strains at least defined (constant strain or stress condition), although not necessarily continuous between elements. A constant stress condition is necessary for convergence since, in the limit, if an element is made infinitesimally small, it will then correctly represent the stress at a point, which is constant. For Euler-Bernoulli bending, a continuity of Ch-1 = C2-1 = C1 (where h is the highest derivative order of the displacement in the governing differential equation) is required. For Timoshenko bending, C0 is sufficient. For plane stress, C0 is sufficient. C0 implies that interelement continuity of displacement is required but not any of its derivatives, hence strains and stresses are not continuous between elements. It has been said that as a mesh of displacement based compatible finite elements is refined, the unknown nodal displacement estimates will converge monotonically. If the form of loading is by point forces or surface pressures, then the finite element solution will converge from a stiffer response to the exact solution in the limit. Conversely, if the loading is in terms of applied displacement or strains (such as support movements or thermal loads), then the finite element response will converge from a more flexible response to the exact solution in the limit. The exact solution of the differential equation satisfies equilibrium and compatibility everywhere. The nature of the finite element solution on the other hand is as follows. (i) (ii) (iii) (iv) (v) (vi) Compatibility satisfies at nodes naturally when the elements are connected at common nodes Equilibrium satisfied at nodes as the equation of static or dynamic equilibrium requires; that for a linear static analysis is {P} = [K] {U} Compatibility satisfied within the elements because of the continuous polynomial interpolation, unless under-integration of the element stiffness matrix is made. Compatibility should be satisfied across inter-element boundaries barring poor user meshing. For compatibility, the displacement function must be continuous across element boundaries, i.e. at least C0 continuity at these boundaries. Inter-element C0 continuity is satisfied for standard TRIA3, TRIA6, QUAD4, QUAD8, HEX8 and HEX20 elements. Compatibility is not satisfied when a QUAD4 is connected to the mid-side nodes of a QUAD8 or a TRIA3 to the mid-side nodes of a QUAD8 and other poorly formed connections or mesh transitions. Note however that QUAD8 connected to a TRIA6 will ensure compatibility. A good mesh transition for refinement is simply to use QUADs (instead of TRIAs) throughout the transition. Equilibrium is usually NOT satisfied within the element Equilibrium is NOT satisfied at or across element boundaries of C0 elements but is across C1 elements. With mesh refinement, the results will converge to the true solution for displacements and stresses. Stress analysis requires a much finer mesh density than static displacement response. This is because of the rate of convergence of displacement response being much greater than that of the stress. 896 Structural Engineering Analysis and Design Second Edition 6.3.2 Finite Element Displacement Interpolation Function, Output Stress Variation, and Corresponding Order of Error in Displacement and Stress Discretization of the continuum structure with appropriate finite elements is crucial. Interpolation function or the shape functions of an element define the variation of displacement within the element. It is of paramount importance to understand the nature of deformations that can be modeled by certain finite elements. For a simple beam element, the axial deformation differential equation is du dx F = AE (Engineers Axial Theory σ = F/A = Edu/dx) The bending deformation differential equation is EI d 2u =M dx 2 (Engineers Bending Theory σ/y = M/I = E/R = Ed2u/dx2) The shear deformation differential equation is du V = dx GA s (Engineers Shear Theory τ = VQ/(Ib) or on average V/As = Gdu/dx) The torsion deformation differential equation is GJ dφ =T dx (Engineers Torsion Theory τ/r = T/J = Gdφ/dx) These are also epitomized in the virtual work (unit load method) expression to find deflections of systems. ∆ 1 = external real kinematic due to unit external real action = f1 ' δ 1 = ∫ (M )  M1  ds  +  EI  R (  P1spring  V  k spring 1 V  + P1spring ∫ = M1 ) ∫ (P )  P1  P L ds  or (P1 )V  1  +  EA  R  EA  R 1 V    + M 1spring  R (   M 1spring  V  k rotational  spring )    + T1spring  R ( ∫ (T )  T1   ds  +  GK t  R 1 V   T1spring  V  k torsional  spring ) ∫ (V )  V1 Q  ds   GIb  R 1 V      R P1sp M 1sp T1sp M1 P PL T VQ ds + P1 1 ds or P1 1 + T1 1 ds + V1 1 ds + P1sp + M 1sp + T1sp EI EA EA GK t GIb k sp k rot sp k tor sp ∫ ∫ ∫ The shear deformation expression is often simplified from VQ/(GIb) to V/(GAs). By definition, EA is the axial rigidity, EI is the flexural rigidity (often denoted D), GAs is the shear rigidity and GJ or GKt is the torsional rigidity (often denoted H). For isotropic materials, G is always E/[2(1+ν)]. 897 Structural Engineering Analysis and Design Second Edition 6.3.2.1 One Dimensional Beam Finite Element Beam elements such as CBAR should only be used if plane sections remain plane and the neutral axis remains strain free. If an open section clearly warps (plane section no longer plane), then shell elements should be used. Apart from that, small deflection theory must be applicable. Beam theory can be based upon the Bernoulli-Euler beam (also known as the classical or engineering beam) or the Timoshenko beam, the latter of which includes shear deformations. Beam elements have in general 6 DOFs in their two end nodes. A 2-noded beam element describes in its displacement vector {y}, a 3rd order complete polynomial transverse displacement = constant + x + x2 + x3 variation in one variable x due to the four (two transverse translational and two rotational) nodal DOFs. Writing the transverse displacement in terms of shape functions (with natural coordinates), the transverse displacement Its strain vector {ε} thus contains a linear variation of curvature (which is defined as the second derivative of the transverse displacement with respect to x along the element). Subsequently, the stress vector {σ} also contains a linear variation of bending moment. Note that the strain for a beam finite element is the curvature and the stress is the bending moment. Note that the required continuity between the finite elements is C2-1 = C1 since the second derivative of the displacement needs to be defined. The second derivative (which is the curvature) and hence the bending moment will thus be continuous between elements. If the bending moment variation is accurate, so will be the shear force distribution, which is the first derivative of the bending moment. A two-noded beam can model concentrated external forces and moments applied at its nodes exactly because the displacement variation will be cubic, the curvature will be parabolic and the bending moment linear. This is the reason that concentrated loads should never be applied within a beam finite element as the resulting bending moment variation will be piecewise linear, a variation that cannot be modeled by a continuous linear function. Likewise a uniformly distributed load within a beam finite element will require at least a quartic (4th order) displacement variation function and parabolic bending moment variation function, both of which cannot be modeled by a two-noded beam element. Note however that a three-noded beam element will be able to model a uniformly distributed variation in internal load 898 Structural Engineering Analysis and Design Second Edition exactly because the resulting displacement variation will be quintic (5th order) and the resulting bending moment variation will be cubic. If the variation in the displacement function or the stress function is not able to model the actual variation in reality (which is dependent upon the variation of the external loads), there will be a discretization error in the finite element approximation. The approximate order of error in the displacement and the strain and stress of a two-noded beam element are given by Displacement Error Order = O(hp+1) = O(h4) Strain (Curvature) / Stress (Bending Moment) Error Order = O(hp-m+1) = O(h2) where h is the element size, p the order of the complete polynomial used in the displacement interpolation and m is the order of the displacement derivative representing the strain. Note that the error is independent of the loading but only occurs if the loading causes a variation which cannot be modeled perfectly by the displacement function. In order to decrease the error, clearly we can employ h-refinement by reducing element size (i.e. increasing the number of elements with the original DOFs still maintained) or employ p-refinement by increasing the order of the complete polynomial. Based on the above orders of errors, it is apparent that finite element analysis is associated with higher accuracy in predicting displacements than in predicting strains and stresses. A 2-noded beam element describes in its displacement vector {y}, a 1st order complete polynomial axial displacement = constant + x variation in one variable x due to the two axial translational nodal DOFs. Its strain vector {ε} thus contains a constant variation of axial strain (which is defined as the first derivative of the axial displacement with respect to x along the element). Subsequently, the stress vector {σ} also contains a constant variation of axial force. Note that the required displacement continuity between the finite elements is C1-1 = C0 since only the first derivative needs to be defined. A two-noded beam can model concentrated external axial forces applied at its nodes exactly (do not apply axial force within element) because the displacement variation will be linear and the axial strain will be constant and the axial stress constant. The approximate order of error in the displacement and the strain and stress of a two-noded bar element are given by Displacement Error Order = O(hp+1) = O(h2) Strain (Axial Strain) / Stress (Axial Force) Error Order = O(hp-m+1) = O(h1) A 2-noded beam element describes in its displacement vector {y}, a 1st order complete polynomial torsional rotation = constant + x variation in one variable x due to the two torsional rotation nodal DOFs. Its strain vector {ε} thus contains a constant variation of torsional strain (which is defined as the first derivative of the torsional rotation with respect to x along the element). Subsequently, the stress vector {σ} also contains a constant variation of torsional moment. Note that the required displacement continuity between the finite elements is C1-1 = C0 since only the first derivative of the displacement needs to be defined. A two-noded beam can model concentrated external torsional moments applied at its nodes exactly (do not apply torsional moment within element) because the torsional rotation variation will be linear and the torsional strain will be constant and the torsional moment constant. The force-displacement relationship of the Timoshenko beam is shown. For the Euler-Bernoulli beam, β is zero.  F1   12 M   6L EI  1   = 3  − 12 F ( ) + β L 1 2    M 2   6L 6L (4 + β )L 2 − 6L (2 − β)   δ1  − 6L (2 − β )L   θ1    12 − 6 L  δ 2   − 6L (4 + β )L2  θ 2  − 12 6L 2  899 β= 12EI GAL2 Structural Engineering Analysis and Design Second Edition 6.3.2.2 Two Dimensional Shell Elements (In-Plane Plane Stress or Plane Strain Membrane Stiffness) Shell elements have in general 5 DOFs in all their nodes. Hence, general shell elements have in-plane stiffnesses (of either plain stress or plane strain) and also transverse bending, shear and torsional stiffnesses. Plate elements by definition have only the transverse bending, shear and torsional stiffnesses. The definition of in-plane stiffnesses is important when the shells map a curved geometry or when the geometry becomes curved as a result of deformations in a nonlinear analysis. In these cases, the transverse loadings are resisted both by transverse bending (and shear) stiffness and also by in-plane stiffnesses. In other words, the membrane and bending actions are coupled in curved shells and when deflections are large in a nonlinear analysis. Note that plane stress elements refer to thin (with respect to the other dimensions) shells such that transverse stresses due to in-plane forces do not develop because the out-of-plane dimension is not constrained such as in plate girder webs. Plane strain elements refer to thick (with respect to the other dimensions) shells such that transverse strains due to in-plane forces do not develop because of the out-of-plane constraint such as the slice of a retaining wall, a dam or a long pipe subjected to internal pressure. The mid-plane of the shell element lies exactly halfway between the two faces. All in-plane loads act along the mid-plane and are symmetric with respect to the mid-plane. All boundary conditions are also symmetric with respect to the mid-plane. A 3-noded triangular shell element (known as a constant strain triangle CST) describes in its displacement vector {y}, a 1st order complete polynomial in−plane u = constant + x + y in−plane v = constant + x + y variation in two variables x, y due to the six (two in-plane displacements at the three nodes) nodal DOFs. Writing the in-plane displacement in terms of shape functions (with natural coordinates) and also including the isoparametric representation of the geometry (i.e. in terms of the shape functions), Its strain vector {ε} thus contains a constant variation of two orthogonal normal strains and one shear strain (which are defined as the first derivatives of the in-plane displacement with respect to x, y and xy respectively within the element). Subsequently, the stress vector {σ} also contains a constant variation of two orthogonal normal stresses and one shear stress. Because of the constant nature of the stresses, 4-noded or 8-noded quadrilaterals or 6-noded triangles are thus recommended in general. Note that the required displacement continuity between the finite elements is C0 since only the first derivative of the displacement needs to be defined. Thus the stress, which is the first derivative of the displacement, will not be continuous between elements. A fine mesh will thus be necessary to model large variations in stress. If the variation in the displacement function or the stress function is not able to model the actual variation in reality (which is dependent upon the variation of the external loads), there will be a discretization error in the finite element approximation. The approximate order of error in the displacement and the strain and stress is given by Displacement Error Order = O(hp+1) = O(h2) Strain / Stress Error Order = O(hp-m+1) = O(h1) 900 Structural Engineering Analysis and Design Second Edition A 6-noded triangular (serendipity) shell element describes in its displacement vector {y}, a 2nd order complete polynomial in−plane u = constant + x + y + x2 + xy + y2 in−plane v = constant + x + y + x2 + xy + y2 variation in two variables x, y due to the six (two in-plane displacements at the six nodes) nodal DOFs. Writing the in-plane displacement in terms of shape functions (with natural coordinates) and also including the isoparametric representation of the geometry (i.e. in terms of the shape functions), Its strain vector {ε} thus contains a linear variation of two orthogonal normal strains and one shear strain (which are defined as the first derivatives of the in-plane displacement with respect to x, y and xy respectively within the element). Subsequently, the stress vector {σ} also contains a linear variation of two orthogonal normal stresses and one shear stress. Note that the required displacement continuity between the finite elements is C0 since only the first derivative of the displacement needs to be defined. Thus the stress, which is the first derivative of the displacement, will not be continuous between elements. A fine mesh will thus be necessary to model large variations in stress. If the variation in the displacement function or the stress function is not able to model the actual variation in reality (which is dependent upon the variation of the external loads), there will be a discretization error in the finite element approximation. The approximate order of error in the displacement and the strain and stress is given by Displacement Error Order = O(h2+1) = O(h3) Strain / Stress Error Order = O(hp-m+1) = O(h2) A 4-noded quadrilateral shell element describes in its displacement vector {y}, a 1st order complete polynomial in−plane u = constant + x + y + xy in−plane v = constant + x + y + xy variation in two variables x, y due to the eight (two in-plane displacements at the four nodes) nodal DOFs. Writing the in-plane displacement in terms of shape functions (with natural coordinates) and also including the isoparametric representation of the geometry (i.e. in terms of the shape functions), 901 Structural Engineering Analysis and Design Second Edition Its strain vector {ε} thus contains εx constant in x but linear in y, εy constant in y but linear in x and γxy linear in x and y, the strains are defined as the first derivatives of the in-plane displacement with respect to x, y and xy respectively within the element. Subsequently, the stress vector {σ} also contains σx constant in x but linear in y, σy constant in y but linear in x and τxy linear in x and y. Note that the required displacement continuity between the finite elements is C0 since only the first derivative of the displacement needs to be defined. Thus the stress, which is the first derivative of the displacement, will not be continuous between elements. A fine mesh will thus be necessary to model large variations in stress. The four-noded shell element is however much better then the three noded shell as the variation of stress within the element is linear in some senses, i.e. although the variation of the normal stress in x is constant in x, it is linear in y. If the variation in the displacement function or the stress function is not able to model the actual variation in reality (which is dependent upon the variation of the external loads), there will be a discretization error in the finite element approximation. The approximate order of error in the displacement and the strain and stress is given by Displacement Error Order = O(hp+1) = O(h2) Strain / Stress Error Order = O(hp-m+1) = O(h1) An 8-noded quadrilateral (serendipity) shell element describes in its displacement vector {y}, a 2nd order complete polynomial in−plane u = constant + x + y + xy + x2 + xy + y2 + x3y in−plane v = constant + x + y + xy + x2 + xy + y2 + xy3 variation in two variables x, y due to the eight (two in-plane displacements at the eight nodes) nodal DOFs. Its strain vector {ε} thus contains εx linear in x but parabolic in y, εy linear in y but parabolic in x and γxy parabolic in x and y, the strains are defined as the first derivatives of the in-plane displacement with respect to x, y and xy respectively within the element. Subsequently, the stress vector {σ} also contains σx linear in x but parabolic in y, σy linear in y but parabolic in x and τxy parabolic in x and y. Note that the required displacement continuity between the finite elements is C0 since only the first derivative of the displacement needs to be defined. Thus the stress, which is the first derivative of the displacement, will be continuous between elements. If the variation in the displacement function or the stress function is not able to model the actual variation in reality (which is dependent upon the variation of the external loads), there will be a discretization error in the finite element approximation. The approximate order of error in the displacement and the strain and stress is given by Displacement Error Order = O(h2+1) = O(h3) Strain / Stress Error Order = O(hp-m+1) = O(h2) 902 Structural Engineering Analysis and Design Second Edition 6.3.2.3 Two Dimensional Shell Elements (Out of Plane Bending, Shear and Torsional Plate Stiffness) 19 The use of solid elements of model thin plates would be extremely expensive unless one of dimensions of the solid is allowed to be very small in comparison to the other two. Thin solids however would be very badly conditioned. Hence the development of plates and shells. By definition plates resist bending, membranes resist in-plane forces and shells resist both bending and in-plane membrane actions. Shell elements have in general 5 DOFs in all their nodes. Hence, general shell elements have in-plane stiffnesses (of either plain stress or plane strain) and also transverse bending, shear and torsional stiffnesses. Plate elements by definition have only the transverse bending, shear and torsional stiffnesses. The definition of in-plane stiffnesses is important when the shells map a curved geometry or when the geometry becomes curved as a result of deformations in a nonlinear analysis. In these cases, the transverse loadings (i.e. normal to the surface) are resisted both by transverse bending (and shear) stiffness and also by in-plane stiffnesses, i.e. coupled membrane-bending behavior. To reiterate, flat plates can behave as membranes with no bending strains or as bending elements with no membrane action when the loading is in-plane or out-of-plane. This would be an incorrect representation of reality in the two cases, namely when the deflections are large in a nonlinear analysis and when the initial undeflected geometry is curved to start with. In these cases, the transverse and in-plane loadings are resisted by both bending and membrane action, i.e. their stiffnesses are coupled. Note that membrane actions is far more efficient than bending action. Resisting loading by bending is generally an inefficient method. For out-of-plane loading, it must be remembered that shell models are used to model thin flat plate structures subjected to transverse loading in reality. Possible mathematical models include: 1. Membrane shell model: for extremely thin plates dominated by membrane effects, such as inflatable structures and fabrics (parachutes, sails, etc). 2. Von-Karman model: for very thin bent plates in which membrane and bending effects interact strongly on account of finite lateral deflections. Important model for post-buckling analysis. 3. Kirchhoff model: for thin bent plates with small deflections, negligible shear energy and uncoupled membrane-bending action. 4. Reissner-Mindlin model: for thin and moderately thick bent plates in which first-order transverse shear effects are considered. Particularly important in dynamics as well as honeycomb and composite wall constructions. 5. High order composite models: for detailed (local) analysis of layered composites including inter-lamina shear effects. 6. Exact models: for the analysis of additional effects using three-dimensional elasticity. The first two models require geometrically nonlinear methods of analyses. The last four models are geometrically linear in the sense that all governing equations are set up in the undeformed flat configuration. The last two models are primarily used in detailed or local stress analysis near edges, point loads or openings. All models may incorporate other types of nonlinearities due, for example, to material behavior, composite fracture, cracking or delamination, as well as certain forms of boundary conditions. The Kirchhoff and Reissner-Mindlin plate models are the most commonly used shells models in statics and vibrations, respectively. The Kirchhoff model requires the thickness dimension h to be everywhere small, but not too small, compared to a characteristic length L of the plate mid-surface. The term “small” is to be interpreted in the engineering sense and not in the mathematical sense. For example, h/L is typically 1/5 to 1/100 for most plate structures. A paradox is that an extremely thin plate, such as the fabric of a parachute or a hot air balloon, ceases to function as a thin plate! The Kirchhoff model also assumes inextensional bending i.e. the plate does not experience appreciable stretching or contractions of its mid-surface. This is simply known as plate bending. The Von-Karman model on the other hand assumes extensional bending, i.e. the mid-surface experiences significant stretching or contraction. This is also called coupled membrane-bending. 19 FELIPPA, Carlos A. Advanced Finite Element Methods. Center for Aerospace Structures, University of Colorado, 2001. 903 Structural Engineering Analysis and Design Second Edition Note that analyzing plate bending as a series of beams bending in two orthogonal directions ignores the role of twisting moment and also the Poisson contractions. The Euler-Bernoulli beam and the Kirchhoff plate model both ignore transverse shear deformations (although the shear force is of course still calculated). The assumptions of these models are that the planes normal to the midsurface remain plane and normal (orthogonal) to the deformed mid-surface. On both the Euler-Bernoulli beam and the Kirchhoff plate, without shear deformation, the required displacement continuity between elements is C1. The Kirchhoff plate uses one parameter to describe the displacement field, for a QUAD4 with 3 DOFs at each node (two out-of-plane rotational and one transverse displacement), w = constant + x + y + x2 + xy + y2 + x3 + y3 + x2y + xy2 + x3y + xy3 which is a complete 3rd order polynomial (incomplete 4th order). Curvature (and stress and moment) would thus be linear like the Euler-Bernoulli beam. But this element is incompatible in normal slope. In fact, Kirchhoff elements generally suffer from the inability to be fully C1 compatible. However, these incompatibilities reduce to zero with mesh refinement and the elements can performs satisfactorily. Another failing of the Kirchhoff elements is that they cannot be generalized to curved side configurations. The Discrete Kirchhoff elements on the other hand use independent displacement and rotation interpolation fields w, θx and θy much like the Mindlin approach which abandons the simple Kirchhoff bending theory altogether. The Timoshenko beam hand includes shear deformation correction terms in its stiffness matrix. In an analogous way, shear correction terms can be included in the Mindlin plate model to represent deeper plates. Here, planes normal to the mid-surface remain plane and but not necessarily normal (orthogonal) to the deformed mid-surface. On both the Timoshenko beam and the Mindlin plate, with shear deformation, the required displacement continuity between elements is C0. Unlike the Kirchhoff plate element which uses just one parameter to describe the displacement field, the Mindlin model uses uncoupled displacement and rotational fields w, θx and θy. Each node still has 3 DOFs (two out-of-plane rotational and one transverse displacement). The curvature is no longer the second derivative of the displacement field, instead the first derivative of the rotation field. Because the highest derivative is only the first derivative, the continuity requirement is only C0. The Mindlin model also automatically results in through-thickness transverse shear strains (unlike the Kirchhoff model which required equilibrium considerations). The Mindlin model is superior to the Kirchhoff model if the plate is thick as the shear deformations become important when the thickness of the plate is greater than about 1/10 of the plate width in a physical sense, not mathematical sense of the element. This is because the Mindlin model represents the shear deformation directly instead of having to infer it as the derivative of the bending moment, the latter of which is more inaccurate. Modelling thin plates with Mindlin elements on the other hand lead to the susceptibility of shear locking (a form of ill-conditioning as the shear strains become relatively insignificant). The condition can be avoided by using reduced integration for the shear stiffness terms whilst the bending stiffness terms can still be fully integrated to avoid spurious modes. Hence a QUAD8 would have a 3 x 3 Gauss rule for bending but only a 2 x 2 for shear. The Mindlin model can also be generalized to curved isoparametric formulations. 904 Structural Engineering Analysis and Design Second Edition 6.3.2.3.1 Kirchhoff Plate Element Like beams, Kirchhoff plate elements are C1 plate elements because that is the continuity order nominally required for the transverse displacement shape functions. The Kirchhoff model is applicable to elastic plates that satisfy the following conditions. (i) The plate is thin in the sense that the thickness h is small compared to the characteristic length(s), but not so thin that the lateral deflection become comparable to h. (ii) The plate thickness is either uniform or varies slowly so that 3-dimensional stress effects are ignored. (iii) The plate is symmetric in fabrication about the mid-surface. (iv) Applied transverse loads are distributed over plate surface areas of dimension h or greater.6 (v) The support conditions are such that no significant extension of the mid-surface develops. The kinematics of a Bernoulli-Euler beam is based on the assumption that plane sections remain plane and normal to the deformed longitudinal axis. The kinematics of the Kirchhoff plate is based on the extension of this assumption to biaxial bending i.e. material normals to the original reference surface remain straight and normal to the deformed reference surface. Material normals, also called material filaments, are directed along the normal to the mid-surface (that is, in the element z direction) and extending h/2 above and h/2 below it. The magnitude h is the plate thickness. As shown on the diagram, the variation of the two orthogonal direct stresses and the one (bending or in-plane, as opposed to transverse) shear stress over the thickness of the element is linear. These thus give rise to moments when integrated. 905 Structural Engineering Analysis and Design Second Edition The Kirchhoff model suffers from 2 inconsistencies. Firstly, the transverse shear strains are zero. If the plate is isotropic and follows Hooke’s law, this implies σxz = σyz = 0 and consequently there are no transverse shear forces. But these forces appear necessarily from the equilibrium equations. Secondly, εzz = 0 says that the plate is in plane strain whereas for plane stress σzz = 0 is a closer approximation to the physics. For a homogeneous isotropic plate, plane strain and plane stress coalesce if and only if Poisson’s ratio is zero. Both inconsistencies are similar to those encountered in the Bernoulli-Euler beam model. As in the case of Bernoulli-Euler beams, predictions of the transverse shear stresses must come entirely from equilibrium analysis. The Kirchhoff plate model ignores the transverse shear energy, and in fact predicts σxz = σyz = 0 from the kinematic equations. In practical terms this means that the transverse shear stresses should be significantly smaller than the bending stresses. If they are not, the Kirchhoff model does not apply, nor does the Bernoulli-Euler beam for that matter. From equilibrium conditions, the transverse shear stresses and hence transverse shear forces can be derived. As indicated on the diagram, the variation of the two transverse shear stresses over the thickness of the element from equilibrium conditions is parabolic, peaking at the neutral axis. These thus give rise to transverse shear forces when integrated. The only term not calculated for plates is the σzz, and hence the Fzz. 906 Structural Engineering Analysis and Design Second Edition 6.3.2.4 Three Dimensional Solid Elements 907 Structural Engineering Analysis and Design Second Edition 6.3.3 6.3.3.1 Finite Element Modelling For Static Analyses Choice of Finite Element to Model the Load Path and Deformation The choice of the finite element whether beams, shells or solids depend on the stiffness (which in turn depends on the geometry) that we are trying to model in reality. Bending deformations govern in beams with span to depth (S/D) ratios greater than 10 and of course finite element beams with shear deformations can be used to analyze and design. When S/D less than 10, shear deformations should be included as well, and finite element beams with shear deformations can be used to analyze and design. The inclusion of shear deformations will correctly decrease the stiffness of the element. For S/D less than 2.5 it becomes a deep beam and thus finite element beams may be used to analyze but deep beam design must be employed. When S/D is less than 1 the section is not a beam, i.e. flexural deformations (and shear deformations do not occur and the load path is much more direct; note that flexural stiffness is much smaller than axial stiffness). This occurs in shear walls where the load path is such that the wall arches instead of bending like a beam. Shear walls should thus be modeled using vertically orientated shells or even simply plane stress membranes when there are no out-of-plane forces. Another example of an S/D less than 1 section is the capping beam of contiguous piles, used for foundations. It is inappropriate to model the capping beam as finite element beams between piles with a very small spacing in between such that they are effectively continuous (hence the name contiguous piles). Solid elements are really the only practical option. Alternatively, if explicit modelling is not required, but simply a good representation of the capping beam stiffness, the section can be made rigid as it does not behave like a beam. This is akin to modelling sections that are far more rigid than adjacent sections as rigid for a global representation, and only then performing a local analysis on the section explicitly modeled if required. The design of the capping beam can then be based on a strut and tie model. Flat thin plates such as flat slabs can be modeled using a mesh of 2D shells (shells encompass both bending plates and in-plane membrane plane stress elements) or simplistically as a grillage of 1D beam elements, which effectively constrains the load paths. Ribbed slabs are best modeled with a combination of shells and beam elements. I-beams, tubes and cylinders can be modeled explicitly using plane stress shell elements. Complicated geometries that do not act like simple beams or thin shells must be modeled with solids. 6.3.3.2 Concepts of Stiffness Concepts of stiffness are crucial in linear static analyses. It is worth noting that the equivalent stiffness of springs in parallel is the addition of the individual stiffnesses and the equivalent stiffness of springs in series is the inverse of the addition of the inverse of the individual stiffnesses. Stiffness in series occurs when the load path has to travel both stiffnesses sequentially. Stiffness in parallel occurs when the load path is given the option to be more attracted to the stiffer element. In series, there is no question of whether the load will travel the path or not, for it must, all loads must travel some path, and in series, there is no other option. Hence, elements of different stiffness in series will all experience the same load effects. In a statically indeterminate system, the elements with a greater stiffness in a particular DOF (with other elements attached to the same DOF, hence in parallel) will attract more force, because they are more resistant to deformation. The parallel members with smaller relative stiffness contribution will conversely attract less force. However, all the load that is applied must eventually be balanced by the reactions at the supports, i.e. all the applied load must be resisted in line the principle of conservation of energy. The statically indeterminate system simply distributes this applied loading according to its distribution of stiffness, eventually to its supports. Let us reiterate that in a linear static analysis, all the applied forces must be balanced by the reactions. Deviations of the sum of the applied loads and the reactions from zero are an indication of ill conditioning. These deviations also occur when there is a loss of internal strain energy. This happens when there is artificial rotational stiffness applied onto the rotational DOFs on 2D shells that do not have their own in-plane rotational stiffness in order that the originally singular equations may be solved. There is thus obviously a loss of accuracy as some of the applied loads are not resisted by the structure but lost into the artificial constraints. 908 Structural Engineering Analysis and Design Second Edition 6.3.4 Finite Element Modelling For Dynamic Analyses Modelling for dynamic analyses involves additional considerations on top of those for static analyses. 6.3.4.1 Mass and Stiffness Distribution A static mesh is usually refined as locations of high stress concentration. A dynamic mesh is often more uniform as the consideration of not only the location of the loading and inherent geometry that cause stress concentrations (as with static analysis), but also the time variation of the loading and the nature of the response of a dynamic analysis where higher modes cause local stress concentrations which are not observed in a static analysis. As a minimum requirement, the lower modes of the structure must have the correct resonant frequencies and mode shapes. The lowest modes of vibration generally involve mode shapes that minimize the strain energy and maximize the kinetic energy. Imagine the natural bending modes of a simply-supported beam. The higher the bending mode, the more the strain energy in the system for a maximum amplitude of displacement. Also, the higher the bending mode, the less the kinetic energy in the system as more points within the beam are stationary. Uniform distributions of mass and stiffness require a uniform mesh. Since minimizing the strain energy requires a detailed description of the stiffness distribution, the stiffness matrix must be as accurate as possible. Generally, a dynamic analysis can have a coarser mesh than a static analysis because the response tends to be controlled by the low frequency behavior, usually much less than 10% of the total number of possible modes is necessary. Areas of low stiffness must be accurately modeled, as these are the areas where deformation is largest and since the stiffness is low, the strain energy will be minimized. Note also that since deformations are high, the kinetic energy will be high, thus giving the two conditions required to simulate low frequency modes accurately. On the other hand, a coarse mass distribution with lumped masses (instead of the more expensive banded kinematically equivalent coupled mass matrix) is generally sufficient as maximizing the kinetic energy is much easier to achieve. More care must be taken with mass description if the higher modes of vibration are required, where coupled mass formulations may be more accurate. Large masses must be correctly positioned in the model. In order to simulate lower modes accurately, to maximize the kinetic energy, the nodes should be positioned where the mass is large. If only the first few resonance frequencies and mode shapes are required, then a relatively coarse mesh can be used. If higher frequencies are required, then the mesh must be suitably fine to model the more complicated mode shapes. A good parameter may be the modal mass. We know that the modal mass of all the bending modes of a beam is half the beam mass if simply supported and quarter the beam mass if a cantilever. When higher modes deviate from the modal mass value, then we know that the mode shape cannot be captured by the mesh. With more complicated structures, an h- or p-refinement should be performed and the modal masses of the original and the refined mesh should be compared; modal masses of higher modes which begin to show discrepancies indicates the extent of the capability of the mesh in capturing these higher modes. Modal eigenvector displacement and frequencies response does not require a very fine mesh. If a dynamic stress analysis is to be performed, then the mesh must be comparably fine to that for a static stress analysis. Acceleration response requires a finer mesh than displacement response, as good accuracy of higher modes is required. 6.3.4.2 Nonstructural Mass The dynamic mass often includes the medium surrounding the structure. For instance, in the analysis of offshore gravity platforms, some degree of the mass of the water surrounding the shafts must be included within the mass. Noting that the mass acts in 3 translational orthogonal directions (likewise inertia acts about 3 orthogonal axes), it is essential that the correct component be modeled. The added mass on the shafts is a horizontal mass component whilst the added mass on the base of the gravity base structure is a vertical mass component. The inclusion of added masses on the dynamic model also means that a uniform global acceleration applied to all parts of the structure to model gravitational force cannot be employed, as the added mass will incorrectly increase the weight of 909 Structural Engineering Analysis and Design Second Edition the structure. Instead, the gravitational force must be modeled using explicit nodal loads or more accurately, gravitational accelerations applied to a set of masses that excludes the added masses. Another important consideration when modelling non-structural mass is that if rigid links are used to model the center of gravity of the non-structural mass from the structure, then a coupled mass formulation (kinematically equivalent mass matrix) must be used. This is because if lumped mass formulation is used, the rigid links simply will transfer the non-structural mass onto the structure, and hence effectively not incorporating the offset. This will cause significant errors in the lowest frequencies. The offset mass increases the rotational inertia and this has the effect of reducing some of the natural frequencies and hence potentially increasing the response. 910 Structural Engineering Analysis and Design Second Edition 6.3.5 Modelling Mechanisms With Inertia Relief – Modelling Displacement Effects Due to Applied Loads On Systems in Conditionally Stable Equilibrium Inertia relief is used to model mechanisms and unconstrained structures in static solutions. The structure is assumed to be in a steady-state condition, i.e. no transient dynamic effects. The displacements obtained will be relative to a moving frame of reference. The inertia (mass) of the structure is used to resist the applied loadings, that is, an assumption is made that the structure is in a state of static equilibrium (steady-state) even though it is not constrained. Examples include a spacecraft in orbit, an aircraft in flight or an automobile on a test track. The method is used to find out what happens to these structures relative to their moving frame of reference (due to their steady-state condition) when an additional excitation is applied. There are two ways to invoke the inertia relief. The first method is to specify the SUPORT entry explicitly by including “PARAM, INREL, -1” in the Bulk Data Section. The second method (the recommended method) is to let MSC.NASTRAN select the SUPORT degrees of freedom automatically by including “PARAM, INREL, -2” in the Bulk Data Section. Either way, all 6 possible rigid body motions must be constrained by SUPORT. An optional “PARAM, GRDPNT, x”—where x is a grid point ID—can be specified in the model. If “PARAM, GRDPNT, x” is used, the loads and accelerations will be summed about this point. If “PARAM, GRDPNT, x” is not specified, then the loads and accelerations will be summed about the origin of the basic coordinate system. When inertia relief is specified, MSC.NASTRAN calculates the forces that result from a rigid body acceleration about the point specified on the “PARAM, GRDPNT, x” in the specified directions. MSC.NASTRAN then calculates the summation of all applied loadings in the same directions. Accelerations are applied to the structure in the appropriate directions to “balance” the applied loadings. The structure is now in a state of static equilibrium, i.e., the summation of all applied loads is 0.0. Since the problem is not constrained, rigid body displacement is still possible. The next step performed by MSC. NASTRAN is to constrain the SUPORT degrees of freedom to a displacement of 0.0 and provide the relative motion of all other grid points with respect to that reference point. Hence, the term “reference” degree of freedom is used to describe the SUPORT degrees of freedom in MSC. NASTRAN. The set of degrees of freedom described on the SUPORT entry belong to the r-set or reference set for the solution. The computed solution is the correct one, and it is relative to any rigid body motion that is occurring. To perform manual inertia relief, the following is undertaken. $ CASE CONTROL SECTION PARAM, INREL, -1 $ BULK DATA SUPORT GID1 C1 GID2 C2 GID3 C3 GID4 C4 The inertia relief method requires that a realistic mass distribution exists, and the degrees of freedom listed on the SUPORT entry must be connected elastically to the model in all specified 6 degrees of freedom. (For example, degrees of freedom 4, 5, and 6 on a grid point with only solid elements attached cannot be used since solid elements have no stiffness in these degrees of freedom). It is good practice (but not required by MSC.NASTRAN) to use the same grid point on PARAM, GRDPNT and on the SUPORT entry. An additional feature allowed in Solution 101 is the solution of a problem under uniform acceleration. This problem is posed using the DMIG, UACCEL Bulk Data entry in addition to the previously mentioned requirements. In this case, uniform accelerations are applied to the model, and the solution is found. Uniform accelerations are useful for situations, such as spacecraft liftoff and landing loadings, which are often specified as static accelerations. 911 Structural Engineering Analysis and Design Second Edition The OLOAD output will present the applied loads and also 6 sections for the loads necessary to impose unit accelerations in the 6 DOFs about the support point. Whenever a SUPORT entry is used in static analysis, the epsilon and strain energy printed in the table from UIM 3035 should be checked. The values printed for epsilon and strain energy in the UIM 3035 table should all be numeric zero. The strain energy printed in this table for matrix KLR represents the strain energy in the model when the one SUPORT degree of freedom is moved 1.0 unit, while all other SUPORT degrees of freedom are constrained. If the SUPORT degrees of freedom are properly specified, the model should be capable of rigid body motion (strain-free) with no strain energy. The values printed for the strain energy indicate the ability of the model to move as a rigid body. These values should always be checked. If the structure is not constrained, the values should be numeric zero, but roundoff almost always results in a small nonzero value. Acceptable values are a function of the units, size of the structure, and precision of the hardware. The element forces and stresses will be zero since it is motion without strain that we are modelling. Hence the SPC forces corresponding to the SUPORT freedoms will also be zero. The displacements of the structure of course will not be zero except at the SUPORT location, hence the displacements are relative to the SUPORT. Note that the elements used in inertia relief must have mass and inertia. Hence CBAR elements may be unreliable at times (when they are collinear), thus it is recommended that CBEAMs used instead. In manual inertia relief, when the r-set is chosen such that structure is not constrained in a statically determinate manner, or if the stiffness attached to these points is inadequate, the rigid body mode shapes may be poor, leading to low accuracy in inertial load calculations. A poor static analysis solution may also result from the poor constraints, independent of the loading problems. Both effects may result in poor overall accuracy. Poor results can occur with little warning when the SUPORT entry is misused. To perform automatic inertia relief, the following is undertaken. $ CASE CONTROL SECTION PARAM, INREL, -2 The specification of a SUPORT entry is no longer required. The reference frame is selected automatically, in a manner that poor solutions are unlikely because of the choice of reference frame variables. The DMIG, UACCEL cannot be used with automatic inertia relief. 912 Structural Engineering Analysis and Design Second Edition 6.3.6 Submodelling Techniques for Static Analysis 20 Submodelling refers to refined analysis of a local area after a global analysis is carried out. This clearly eliminates the need for a refined global mesh or a complicated transition to a refined mesh whilst saving computational effort. Substructuring on the other hand, refers to a procedure that condenses a group of finite elements into one element called a superelement. The computational effort for is greatly reduced if the superelement is used within a structure instead of all the individual elements. Submodelling can (and should) be performed using substructuring techniques such as static condensation using superelements (for the remaining parts of the structure), but, in practice, other alternative techniques are used for linear static analysis. These alternatives are boundary internal forces and boundary enforced displacements techniques. When local analysis is to be performed in a zone of a structure that probably is going to be modified (thickness increments, local reinforcements, etc) from local analysis results (stresses, displacements), the best approach to set appropriate boundary conditions is using the substructuring technique of static condensation with MSC.NASTRAN superelements for the remaining parts of the structure. This technique will give exact results. Boundary internal forces and enforced displacements methods will be inappropriate, specially, when large stiffness modifications are foreseen in local model, or when local fine model stiffness is substantially different from the stiffness of local zone modelling used in the complete model. To reiterate, the substructuring technique using superelements is exact for local modelling. That is to say, the rest of the structure is reduced to superelements, whilst local mesh and design changes are performed on a local part. These local analyses may refer to local stress analysis, local redesign iterations, local buckling analysis and local non-linearity analysis. Submodelling by substructuring using superelements is also mandatory when different components of a whole model strategically and confidentially shared between several companies (i.e. aircrafts, engines and space structures). 6.3.6.1 Submodelling by Substructuring – Static Condensation (Guyan Reduction) using Superelements Very often, in a complicated structure, some sort of manual substructuring is required. Different parts of the structure will be analyzed separately. All the applied loads must eventually find their way to the constraints. For instance, in large structural engineering projects where a multiple story building structure is to be analyzed, the higher stories may be analyzed separately from that below. The higher story may incorporate a shear wall as a structural load-resisting element being rested upon say a beam in the story below. It will be incorrect to restrain rigidly all the supports of the higher story, i.e. the base of the shear wall must not be all supported on rigid supports (with the intention of applying the reaction forces onto the beam of the story below in the opposite direction). If this was done, the shear wall would not arch, but all the load would simply transfer straight down into the rigid supports. Hence, instead, the relative support stiffness under the shear wall must be incorporated, by say modelling the beam as well. The shear wall will then arch and the load distribution will be far more realistic with more of the load transferring directly to the supports of the shear wall. The reactions on these flexible supports (here the forces on the beam and the ends of the shear wall) can then be transferred onto the model containing the story below. If on the other hand, had all the load-resisting elements been columns supported on equal stiffness foundations, the supports of the upper story could well have been rigid and the reaction applied onto the story below. To model the boundaries of the local model with appropriate stiffness is substructuring. Here we have performed manual substructuring as the stiffness of the remaining part of the structure was approximated manually. To sum up, when manual substructuring is undertaken, the supports of a substructure should be modeled to incorporate their relative stiffness such as to obtain the correct distribution of reactions, which in turn will be applied (of course in the opposite direction – Newton’s Third Law) onto the model containing the adjacent substructure. This of course is an approximate procedure as the substructuring is performed manually. Automatic substructuring using superelements to provide the stiffness at the boundaries of the local model is on the other hand exact. 20 MATINEZ, Angel. Submodelling Techniques for Static Analysis. MSC. Software First South European Technology Conference, 7-9 June 2000. 913 Structural Engineering Analysis and Design Second Edition Modelling the stiffness of the adjacent (to the substructure) elements is fundamental to substructure analysis. The static condensation technique does just that by reducing the equations to only involve the DOFs of the substructure and its interface, but in doing so incorporates the stiffness and internal forces of the remaining part of the whole model onto the interface DOFs. The most important characteristic of static condensation is that the boundary conditions at the interface of the substructure depends only on the stiffness and the loading of the remaining part of the whole model and is totally independent of the stiffness and loading of the submodel. Hence any modifications to the loading and stiffness of the submodel are perfectly acceptable and the answers will be exact. Thus, for static analysis, the static condensation technique produces the exact same results as that obtained from the full analysis. Consider a finite element model of a structure that has been properly constrained and loaded. Total number of d.o.f.’s is denoted as g, normally equal to 6x(number of nodes). This g set can be subdivided in c (constrained) and Fs f (free). Fm g c f m s m After applying constraint conditions, static analysis equations become in matrix form as follows: [K ff ] ⋅ {δ f } = {Ff } (1) Free (f) d.o.f.’s are going to be subdivided in two sets: m (masters) and s (slaves). Masters d.o.f.’s are the ones to be kept in the reduction process, and slave set will be reduced. This partition gives expression (1) the following form: K mm K  sm K ms  δ m  Fm  ⋅  =   K ss   δ s   Fs  (2) that results in these two equations: [K mm ] ⋅ {δ m } + [K ms ] ⋅ {δs } = {Fm } [K sm ] ⋅ {δ m } + [K ss ] ⋅ {δs } = {Fs } Solving (3) {δ s }from second equation of (3) gives: {δ s } = [K ss ]−1 ({Fs } − [K sm ] ⋅ {δ m }) (4) This expression can be used for the recovery calculation of {δ s }, when {δ m } were known. Considering last expression (4) in first equation of (3), and reordering terms, the following system of equations is obtained: [K mm ] − [K ms ][K ss ]−1 [K sm ] ⋅ {δ m } = {Fm } − [K ms ][K ss ]−1 {Fs } (5) that can be expressed in the compact form: ( ) [K ]⋅ {δ *s mm m } = {Fm*s } (6) being: 914 Structural Engineering Analysis and Design Second Edition [K ] = [K ] − [K ][K ] [K {F }= {F } − [K ][K ] {F } −1 *s mm *s m mm ms ss sm ] (7) −1 m ms ss s [K ] is named reduced stiffness matrix and {F } the reduced load vector. Equation (6) represents the reduced *s mm *s m equations system to master d.o.f.’s set (m). Solving this system, displacements {δ m } at masters are obtained. Expression (4) can be used then, to obtain displacements at slave d.o.f.’s (s). Static condensation applied to linear static analysis gives an exact solution, equal to the solution of the global equation system (2). Consider a finite element model of a structure that is subdivided in two parts or substructures A and B. Finite element model can be subdivided in the following d.o.f.’s sets: • a: internal d.o.f.’s of substructure A. • b: internal d.o.f.’s of substructure B. • i: interface d.o.f.’s between substructures A and B. Fa Fa Fi a Fi a i i b i A Fb b Fb B Stiffness matrices of each substructure take the form:  K iiB K ib  K ai  K (8) K A =  aa K =   B  A  K ia K ii  K bi K bb  Assembling the stiffness matrices of each substructure results in the global system of equations for static analysis of the whole structure: 0  δ a  Fa  K aa K ai K      (9)  ia K ii K ib  ⋅  δi  =  Fi       0 K bi K bb  δ b  Fb  being: K ii = K iiA + K iiB (10) Static reduction is going to be applied to set (b) as slave d.o.f.’s and (a+i) as masters. Stiffness matrix and load vector are partitioned in the following way: K aa K  ia  0 0  K K ib  =  mm K K bb   sm K ai K ii K bi K ms  K ss   Fa     Fm   Fi  =    F   Fs   b (11) Recovering the expressions (7) for the calculation of reduced stiffness matrix and reduced load vector: [K ] = [K ] − [K ][K ] [K {F } = {F } − [K ][K ] {F } −1 *s mm *s m mm ms ss sm ] −1 m ms ss s Applying these equations from established partitions in (11): 915 Structural Engineering Analysis and Design Second Edition [K ] = KK *b ( a +i ) { F(*ab+i ) } K ai   0  −1  − K  [K bb ] [0 K bi ] K ii   ia  ib  0 F     −1 =  a  −   [K bb ] {Fb } K F  i   ib  aa (12) that result in: [K ] = KK *b ( a +i ) { F(*ab+i ) }   K ii − K ib ⋅ K −bb1 ⋅ K bi  K ai aa ia (13) Fa   =  −1 Fi − K ib ⋅ K bb ⋅ Fb  Decomposing each matrix as sum of two terms: [K ] = KK K ai  0 0  = K A + K *iib  A +  B −1  ia K ii  0 K ii − K ib ⋅ K bb ⋅ K bi  (14) 0  Fa  Fa   *b *b F( a +i ) =   +   =   + Fi −1  0  Fi − K ib ⋅ K bb ⋅ Fb   0  The reduced equations systems to d.o.f.’s set (a+i) has the following form: *b ( a +i ) { (K aa } A ) δ  F  + K *iib ⋅  a  =  a  + Fi*b δi   0  (15) [K ]⋅ δδ  = {F } *b ( a +i ) a *b ( a +i )  i (16) Reduced stiffness matrix is composed of the stiffness matrix of substructure A and the reduced stiffness matrix of substructure B to the interface d.o.f. (set i) expanded (completed with zeros) to (a+i) size. In the same way, reduced load vector is the applied load to internal d.o.f.’s of substructure A (set a) plus the reduced load vector of substructure B to set i, and expanded, again, to (a+i) size. In other words, to perform a local static analysis of substructure A by static condensation technique, the following items are needed: • Finite element model of substructure A. • The effect of substructure B over A at interface d.o.f.’s: • Reduced stiffness matrix of substructure B to interface d.o.f.’s (set i), and • Reduced load vector of substructure B to interface d.o.f.’s (set i) Fa A a i [K ] = [K ] − [K ][K ] [K {F }= {F } − [K ][K ] {F } *b ii *b i −1 B ii ib bb bi ] −1 i ib bb b Static Condensation Submodelling Method for Substructure A 916 The most important characteristic of submodelling analysis by substructuring using static condensation is that the boundary conditions at the interface (reduced model of substructure B) only depends on the stiffness of substructure B, and is totally independent of the stiffness of substructure A. Then, any modification of substructure A will be treated correctly, and the results will be the same than the ones obtained with the complete model. Structural Engineering Analysis and Design Second Edition Let us discuss in terms of a-sets and o-sets. Displacement vector sets in NASTRAN define the equations of motion and are partitioned in the following ways. (i) g-set is the unconstrained set of structural equations (ii) the g-set is partitioned into the m-set pertaining to the dependent set of DOFs and the n-set pertaining to the independent set of DOFs g-set − m-set = n-set (iii) the n-set is then partitioned into s-set pertaining to the constrained DOFs and the f-set pertaining to the unconstrained DOFs n-set − s-set = f-set (iv) the f-set is partitioned into the o-set pertaining to the DOFs eliminated by static condensation and the a-set pertaining to the a-set (analysis set) pertaining to the DOFs not eliminated by static condensation f-set − o-set = a-set In the static condensation process you select a set of dynamic DOFs called the a-set; these are the retained DOFs that form the analysis set. The complementary set is called the o-set and is the set of DOFs that are omitted from the dynamic analysis through a reduction process. The process distributes the o-set mass, stiffness, and damping to the a-set DOFs by using a transformation that is based on a partition of the stiffness matrix (hence the term static condensation). This reduction process is exact only for static analysis, but leads to approximations in the dynamic response. The a-set DOFs are defined by the ASET or ASET1 Bulk Data entries, and the o-set DOFs are defined by the OMIT or OMIT1 Bulk Data entries. If you start with the stiffness equation in terms of the set of the unconstrained (free) structural coordinates, you have Partitioning the free degrees of freedom into two subsets of the f-set, you obtain Rewriting On expansion of top equation On expansion of bottom equation First, the f-set is reduced to the a-set using Guyan reduction. Second, the analysis set {ua} is solved for. Third, the omitted set {uo} is solved for. In static analysis, the results using static condensation are numerically exact. The partitioned solution merely changes the order of the operations of the unpartitioned solution. Guyan reduction has special applications in dynamic analysis. In dynamic analysis, the reduction is approximate; the term {uOO} is ignored in this case. The reduction is based solely on static transformation BUT is EXACT provided that no loads are applied to the o-set degrees of freedom. 917 Structural Engineering Analysis and Design Second Edition To utilize static condensation, you can choose either the ASET/ASET1 or the OMIT/OMIT1 entries. With these entries you should specify only the a-set (with ASET/ASET1 entries) or o-set (with OMIT/OMIT1 entries) degrees of freedom. The unspecified remaining f-set DOFs are automatically placed in the complementary set. However, if you specify both the a-set and o-set DOFs, then the unspecified remaining f-set DOFs are automatically placed in the o-set. The same DOF cannot be specified on both the a-set and o-set; otherwise, the job fails with UFM 2101A. Since the reduction process is performed on an individual degree of freedom, it is possible to have some of the degrees of freedom at a grid point in the a-set and other degrees of freedom at a grid point in one of the other mutually exclusive sets. No additional user input is required. $ BULK DATA ASET G1 C1 G2 C2 G3 C3 G4 C4 ASET1 C G1 G2 G3 G4 G5 G6 G7 G8 G9 G10 G11 …etc… C G1 THRU Gi OMIT G1 C1 G2 C2 G3 C3 G4 C4 OMIT1 C G1 G2 G3 G4 G5 G6 G7 G8 G9 G10 G11 …etc… C G1 THRU Gi ASET1 $ BULK DATA OMIT1 The choice of whether to use the ASET/ASET1 or OMIT/OMIT1 is really a matter of convenience. 918 Structural Engineering Analysis and Design Second Edition 6.3.6.2 Submodelling – Boundary Internal Force Method Other way to perform local analysis of substructure A is isolating it and considering internal loads from substructure B to A, as applied loads at interface (set i). Equations system that reflects this approach can be derived reordering terms in expression (15): K aa K  ia K aa K  ia K ai  δ a  Fa   0  = +  A⋅ B −1 −1 K ii   δ i   Fi  − K ii − K ib ⋅ K bb ⋅ K bi ⋅ δ i − K ib ⋅ K bb ⋅ Fb  K ai  δ a  Fa  ⋅ = + F K iiA   δ i   Fi  BA ( ) (17) FBA being the internal loads from substructure B to substructure A. These internal loads are the sum of two terms: • ′ : Action forces over interface when substructure B is constrained (with zero displacement) at interface FBA d.o.f.’s and loaded with its applied load Fb:  K iiB  K bi ′  K ib   0  − FBA  ⋅ = K bb  δ′b   Fb  (18) δ′b = K −bb1 ⋅ Fb ′ = − K ib ⋅ K −bb1 ⋅ Fb FBA • ′′ : Action forces over interface when substructure B is enforced at interface with prescribed displacements FBA δi: ′′   K iiB K ib   δi  − FBA    ⋅  ′′  =  K bi K bb  δ b   0  (19) δ′b′ = −K −bb1 ⋅ K bi ⋅ δi ′′ = −(K iiB − K ib ⋅ K −bb1 ⋅ K bi ) ⋅ δi FBA This term is dependent on displacements at interface d.o.f.’s (set i), and, indirectly, dependent on stiffness changes of substructure A. This means that any stiffness modification in substructure A will imply a perturbation of displacements δi, and then, changes in internal forces FBA. This lead to an important conclusion: there is an inherent inaccuracy in local analysis of substructure A, using internal forces method when stiffness changes are performed in this substructure A. ′ + FBA ′′ As can be seen, it is demonstrated that FBA = FBA (20) In this internal forces approach, it is possible that substructure A has not sufficient constraint conditions to avoid rigid body motions or local mechanism problems. In this case, additional constraints are needed to remove these singularities from stiffness matrix, but their reactions should be equal to zero. In the case that substructure A has no external constraints, an isostatic (statically determinate) set of constraints should be applied. Reactions at these constraints will be zero (or close to zero if the geometry is accurate and there are no significant Poisson effects along the constrained boundary in 2D and 3D models) because FBA, Fa and Fi loads should be in static equilibrium. Fa A a i ( Internal forces at interface ) FBA = − K iiB − K ib ⋅ K −bb1 ⋅ K bi ⋅ δ i − K ib ⋅ K −bb1 ⋅ Fb 919 Internal Forces Submodelling Method for Substructure A Structural Engineering Analysis and Design Second Edition Consider the following pinned base portal frame to submodel. The whole model BMD, SFD and AFD is presented. To submodel half the frame and produce the same internal effects, we need to apply the GPFORCE (in opposite direction) at the interfaces and ensure by applying constraints that the submodel is statically determinate. Encastre The reactions at the artificial encastre support will be found to be ALL ZERO because the free-body is in static equilibrium from the applied forces. Even if the chosen encastre node been the base i.e. the interface, the correct effects will be obtained. The moment reaction at the base will be found to be ZERO as the translational restraints in X and Z equilibrate the applied forces. This method is of course accurate here since the stiffness of the local model has not been altered. If the local model stiffness had been altered, the boundary force method will be inexact. From a practical viewpoint, this is because the stiffness change causes forces to distribute differently. For instance, if the local model stiffness is reduced dramatically, more of the force will distribute to stiffer parts of the structure and carried into the ground. A special case occurs when the remaining part of the structure is isostatically mounted upon the local model (here if the portal frame was a cantilever), in which case changes in stiffness of the local model will still produce exact results as that of the global model. 920 Structural Engineering Analysis and Design Second Edition Encastre In order to obtain the forces acting upon an element (be it a beam, shell or solid), the (global coordinate) grid point forces on the grid for the relevant element is used. Do not confuse grid point stresses with grid point forces. They differ totally in concept. Grid point stresses are the average (global coordinate) stress values at a grid due to element stresses in the (shell and solid) elements adjacent to the grid. Hence, direct (say positive tensile) global coordinate stresses in X in adjacent elements will be averaged to yield a positive tensile global stress at the grid point. The grid stress can be thought of in the same way as the element stress, in the sense that that is the element (global coordinate) stress at that location had there been an element there at the grid. Grid point forces on the other hand are not average forces from adjacent elements. The grid point force balance provides insight into how the loads at a grid are distributed amongst its adjoining elements i.e. it provides information of the load path. The specification of a grid point forces must always be associated with an element (or applied load or reaction). Grid point forces are the global coordinate force acting on a grid due to an adjacent (beam, shell or solid) element. It is NOT THE FORCE ACTING ON THE ELEMENT, BUT ON THE GRID. If all the elements attached to a grid are considered, then the grid point force should theoretically be zero for equilibrium at the grid connection, hence the grid point force balance. Grid point force balance is computed only from linear stiffness elements, the sum of applied loads and thermal loads, and SPC forces. Since GPFORCE is the force acting on the grid (or the structural joint between adjacent elements), it is opposite to the direction of the force acting on the element. Hence, the direction of the GPFORCE from the applied load is the same as the direction of load application, the direction of the GPFORCE from the SPC reaction is the same as the direction of the reaction and the direction of the GPFORCE from an element is opposite the force that acts upon the element. GPFORCE Element in Tension GPFORCE Effects NOT accounted for include those from mass elements in dynamic analysis (inertia loads), rigid elements and MPCs (MPCFORCES), general elements, DMIG entries, and boundary loads from upstream superelements. These effects may lead to an apparent lack of equilibrium at the grid point level. The global coordinate grid point forces for each relevant entity (be they beams, shells, solids, applied loads or SPCs) acting on the grid at each grid is obtained from GPFORCE (PRINT) as follows. 921 Structural Engineering Analysis and Design Second Edition 6.3.6.3 Submodelling – Boundary Internal Force Method of Substructure Isostatically Mounted Over Rest of Structure Suppose a structure composed of two substructures: A and B; substructure B is isostatically mounted over substructure A and has not any external constraints. That is, interface set is a congruent set of six d.o.f.’s that removes rigid body motions of substructure B. Fb B Fi b i Fa Internal Forces Submodelling Method for Substructure A a A Interface forces FBA can be obtained directly from static equilibrium equations and do not depend on stiffness of substructure A or B. In this case, static analysis of substructure B can be performed simply considering constrained to zero its six interface d.o.f.’s:  K iiB  K bi K ib   0  − FBA   ⋅ = K bb  δ b   Fb  FBA = − K ib ⋅ K −bb1 ⋅ Fb = ϕib ⋅ Fb (23) (24) Internal forces (actions over interface) FBA are independent on substructure B stiffness: ϕib matrix is the rigid body modes matrix. This rigid body matrix can be obtained by means of a set of six enforcing displacements conditions that in matrix form corresponds to a unit matrix I:  K iiB  K bi K ib   I ii  Tii  ⋅ =  K bb  ϕib   0  (25) From this equation, it is demonstrated that displacements at internal d.o.f.’s of substructure B correspond to rigid (26) body modes matrix: ϕib = − K ib ⋅ K −bb1 . Other important consideration of equations system (25), is that, by definition, elastic forces Tii necessary to perform rigid body motions should be zero. From this expression (25) the calculation of elastic forces is as follows: Tii = K iiB − K ib ⋅ K −bb1 ⋅ K bi = [0] = K *iib (27) Last expression states an important conclusion: reduced stiffness matrix of substructure B to an isostatic interface is zero. In order words, just in this case in which interface between substructures A and B is isostatic, local analysis (with stiffness modifications) of substructure A can be exactly performed by static condensation or internal forces methods, because these approaches are now identical. 922 Structural Engineering Analysis and Design Second Edition 6.3.6.4 Boundary Enforced Displacement Method Other submodelling technique to analyse locally substructure A consists in enforce displacements δi at interface d.o.f.’s (set i), considering also the applied forces Fa at the internal d.o.f.’s (set a). K aa K  ia K ai  δ a   Fa  ⋅ =  K iiA   δ i  R i  (21) First equations system from above expression gives the static solution for substructure A: K aa ⋅ δ a = (Fa − K ai ⋅ δ i ) (22) External force term in expression (22) is dependent on displacements at interface d.o.f.’s (set i), and, on stiffness changes of substructure A (Kai). This means that any stiffness modification in substructure A will imply a perturbation of this external force term. This lead to the same important conclusion again: there is an inherent inaccuracy in local analysis of substructure A, using enforced displacements method when stiffness changes are performed in this substructure A. Fa A a i Enforced displacements at interface : δi Enforced Displacements Submodelling Method for Substructure A 923 Structural Engineering Analysis and Design Second Edition 6.3.6.5 Numerical Example of Submodelling 6.3.6.5.1 Example 1 – No Local (Substructure A) Stiffness Modification To emphasize the application of submodelling methods, herein it is presented a simple example of structure divided in two substructures. Substructure to be locally analyzed is A. Substructure B Substructure A 10 10 1 2 5 3 5 20 10 60 20 4 Global structure analysis is performed and solved with the following system of equations: 0  δ 2  − 20 δ 2   4   30 − 10 − 10   δ   6    − 10 15  0 − 5  δ 3   0   3    ⋅ = ⇒   =  − 10 0 30 − 20 δ 4   0  δ 4   8       δ5  10 − 5 − 20 25  δ 5   60   0 Example 1 – No Local (Substructure A) Stiffness Modification: Substructuring Using Static Condensation Performing static condensation of substructure B:  30 − 10 − 10 (2)  K bb K bi   KB =  10 0  (3) B  =  − 10 K K ii   ib − 10 0 10  (4) [K ] = [K ] − [K ][K ] [K ] {F }= {F } − [K ][K ] {F }  1 [K ] = 100 100  − −− 10 ⋅ ⋅ [− 10 10 30 *b ii *b i *b ii {F } *b i −1 B ii ib bb bi −1 i ib bb b  2 − 1 (3) − 10] = 10  3  − 1 2  (4)     0  − 10 1 1 (3) =  − ⋅ ⋅ {− 20} = − 20    3 1 (4) 0  − 10 30 Now, local analysis of substructure A, considering static condensation of B, is performed:   K iiA K ia   K *iib 0  δ i   0  Fi*b   +    =   +    K K 0 0 ai aa   δ a  Fa   0    Establishing system of equations and solving:  5 0 −5   2 − 1 0   δ 3   0  1 δ   6        20    3    10    20 − 20 +  − 1 2 0  δ 4  =  0  − 1 ⇒ δ 4  =  8   0   − 5 − 20 25  3  0 0 0  δ  60 3 0 δ  10     5       5    Displacement results for substructure A are the same than those obtained from global structure as expected. 924 Structural Engineering Analysis and Design Second Edition Example 1 – No Local (Substructure A) Stiffness Modification: Internal Forces Method K iiA   K ai K ia   δ i   0  − K *iib ⋅ δ i + Fi*b     =   +  K aa  δ a  Fa   0  ( )  2 − 1 6 − 20 1 − 20 − K *iib ⋅ δ i + Fi*b = − 10  + = 3 − 1 2  8  3 1 − 40       0 − 5  δ3  − 20 5     0 20 − 20 δ 4  = − 40  − 5 − 20 25  δ5   60  Above system of equations has a singular stiffness matrix and cannot be solved. A restraint condition is needed: considering δ4 = 8, the rest of displacements can be calculated, resulting in: δ 3   6      δ 4  =  8  δ  10  5   that are, again, the expected displacement results in substructure A. Example 1 – No Local (Substructure A) Stiffness Modification: Enforced Displacement Method K aa ⋅ δ a = (Fa − K ai ⋅ δ i ) 6 25 ⋅ δ 5 = 60 − [− 5 − 20]  8 That gives δ5= 10, the same expected results. 925 Structural Engineering Analysis and Design Second Edition 6.3.6.5.2 Example 2 – Local (Substructure A) Stiffness Modification Suppose that substructure A is changed to the following configuration: Substructure A 5 3 5 4 60 10 Global structure analysis is performed and solved with the following system of equations: δ 2   4   30 − 10 − 10 0  δ 2  − 20   δ   6.4   − 10 15   0 − 5  δ 3   0   3    ⋅  =  ⇒   =  − 10 0 δ 20 − 10 δ 4   0  7 . 6  4             δ δ 0 − 5 − 10 15 60 11 . 2    5    5  Example 2 – Local (Substructure A) Stiffness Modification: Substructuring Using Static Condensation Local analysis of substructure A considering static condensation of B   K iiA K ia   K *iib 0  δ i   0  Fi*b   +    =   +    K K 0 0 ai aa   δ a  Fa   0     Establishing system of equations and solving:  5 0 −5  2 − 1 0   δ 3   0  1  δ   6.4        20    3   10     10 − 10 + − 1 2 0  δ 4  =  0  −  0 1  ⇒ δ 4  =  7.6  3        − 5 − 10 15  3  0  0 0  δ 5  60   0 δ 5  11.2  Displacement results for substructure A are exactly the same than those obtained from global structure as expected. We shall demonstrate a worked example using static condensation with MSC/NASTRAN superelement capabilities. First, perform static condensation run of substructure B, using DMIGOP2 option. SOL 101 TIME 5 DIAG 14 CEND TITLE = DMIGOP2, RUN 1 PARAM,EXTOUT,DMIGOP2 SPC=1 LOAD=1 BEGIN BULK ASET1 1 3 GRID 1 GRID 2 GRID 3 GRID 4 4 0. 1. 2. 2. 0. 0. 1. 0. 0. 0. 0. 0. 926 Structural Engineering Analysis and Design Second Edition CELAS2 CELAS2 CELAS2 SPC1 SPC1 SPC1 SPC1 FORCE ENDDATA 1 2 3 1 1 1 1 1 10. 10. 10. 123456 23456 23456 23456 2 1 2 2 1 2 3 4 1 1 1 2 3 4 1 1 1 -20. 1. 0. 0. From this run a fort.30 file is output with binary output2 format, containing reduced stiffness matrix and reduced load vector at interface d.o.f.’s declared in ASET1 card. Next perform local analysis of substructure A. ASSIGN INPUTT2='fort.30',UNIT=30 SOL 101 TIME 5 CEND TITLE = DMIGOP2, RUN 2 SPC=1 SUBCASE 1 SUPER=10,1 SUBCASE 2 DISP=ALL SUPER=20,1 LOAD=1 SUBCASE 3 SUPER=0,1 LOAD=1 BEGIN BULK PARAM EXTUNIT 30 SEBULK 10 EXTERNAL BEGIN SUPER=10 $ Substructure B (external superelement) EXTRN 3 1 4 1 GRID 3 2. 1. 0. GRID 4 2. 0. 0. BEGIN SUPER=20 $ Substructure A GRID 3 2. 1. 0. GRID 4 2. 0. 0. GRID 5 3. 0. 0. CELAS2 4 5. 3 1 5 CELAS2 5 10. 4 1 5 SPC1 1 23456 3 SPC1 1 23456 4 SPC1 1 23456 5 FORCE 1 5 60. 1. ENDDATA 1 1 0. 0. Internal d.o.f.’s displacements of substructure A and interface d.o.f.’s displacements are output in F06 file: DATA RECOVERY FOR SUPERELEMENT DMIGOP2, RUN 2 20 IS NOW INITIATED. MAY 5, 2000 D I S P L A C E M E N T POINT ID. 3 4 5 TYPE G G G T1 6.400000E+00 7.600000E+00 1.120000E+01 T2 .0 .0 .0 T3 .0 .0 .0 MSC.NASTRAN 10/11/99 PAGE SUPERELEMENT 20 , SUBCASE 2 V E C T O R R1 .0 .0 .0 927 R2 .0 .0 .0 R3 .0 .0 .0 24 1 Structural Engineering Analysis and Design Second Edition Example 2 – Local (Substructure A) Stiffness Modification: Internal Forces Method 0 − 5  δ 3  − 20 5     0 10 − 10 δ 4  = − 40  − 5 − 10 15  δ 5   60  Above system of equations has a singular stiffness matrix and cannot be solved. A restraint condition is needed: considering δ4 = 8, the rest of displacements can be calculated, resulting in: δ 3   8      δ 4  =  8  δ  12  5   that are incorrect and clearly different than expected. Example 2 – Local (Substructure A) Stiffness Modification: Enforced Displacement Method K aa ⋅ δ a = (Fa − K ai ⋅ δ i ) 6 15 ⋅ δ 5 = 60 − [− 5 − 10]  8 That gives δ5= 11.333, that is, again, an incorrect result. 928 Structural Engineering Analysis and Design Second Edition 6.3.6.6 Static Submodelling Methods Summary Three static submodelling methods are suggested, namely internal force method, enforced displacement method and static condensation substructuring using superelements. The internal force method applies cut boundary forces at all the cut boundaries of the submodel, constraining the submodel anywhere really such that it is just statically determinate. The reactions will be found to be zero (or close to zero if the geometry is accurate and there are no significant Poisson effects along the constrained boundary in 2D and 3D models) because the submodel is subject to a self-equilibrating set of forces. The limitation is only that changes in stiffness of the submodel (due to design geometry or material changes or simply due to the fact that the stiffness will change from the global model to the local model) will produce inaccuracies in the solution. Physically, this is so because if you change the local stiffness of the submodel, the force will either be more attracted or less attracted depending on whether you increase the stiffness or decrease it. A special case occurs when the rest of the structure is ‘isostatically mounted upon the submodel’ i.e. for instance a tree where the submodel is the trunk and the rest of the structure is the branches. In this special case, the internal force method will be exact. The enforced displacement method applies cut boundary displacements at all the cut boundaries of the submodel. No further constraints are required as the submodel will probably no longer be singular due to the application of the enforced displacements, failing which it is perfectly acceptable to constrain the mechanisms such that the submodel is statically determinate. Again the reactions will be found to be zero because the submodel is self-equilibrating. St. Venant’s principle states “if an actual distribution of forces is replaced by a statically equivalent system, the distribution of stress and strain is altered only near the regions of load application. This implies that stress concentration effects are localized around the concentration; therefore, if the boundaries of the submodel are far enough away from the stress concentration, reasonably accurate results can be calculated in the submodel”. Because the submodel will usually be of a finer mesh density, it becomes necessary to interpolate displacements from those at known points along the cut boundaries to all the nodes along the cut boundaries. The limitations of the enforced displacement method is the same as that as for the internal force method, being that inaccuracies are introduced when stiffness changes are made to the submodel. The substructuring method using the static condensation capability of superelements reproduces the exact state of stress and displacements in the local model compared to that of the global model. Apart from refined stress analysis on the detailed local model, stiffness modifications can be made to the local model for local redesign iterations, investigation into local buckling analysis and the modelling of localized non-linearity (to the submodel) can be made. The exact solution is obtained so long as the rest of the structure is modeled with superelements. The stiffness (and internal forces) of the rest of the structure is contained within the superelements, hence it is like modelling the entire structure, only that computationally it is far more efficient. 929 Structural Engineering Analysis and Design Second Edition 6.3.7 6.3.7.1 Submodelling Techniques for Dynamic Analysis Submodelling by Substructuring - Static Condensation (Guyan Reduction) using Superelements For linear dynamic analysis, the static condensation technique is only an approximation (unlike linear static analysis where it is exact) of the whole structure behaviour, and methods with highest efficiency are the ones based on modal synthesis. However, static condensation becomes exact for dynamic analysis if there are no loads applied onto the o-set DOFs, i.e. the set of freedoms omitted by static condensation. 6.3.7.2 Submodelling by Substructuring - Generalized Dynamic Reduction (GDR) using Superelements Generalized dynamic reduction (GDR) offers a more accurate solution by including an approximation of the dynamic effects when forming the transformation. Bulk Data entries for GDR are DYNRED, QSET, and QSET1, and SPOINT. In addition, the Case Control command DYNRED is also required. 6.3.7.3 Submodelling by Substructuring - Component Mode Synthesis (CMS) using Superelements Component mode synthesis (CMS) is a form of superelement dynamic reduction wherein matrices are defined in terms of modal coordinates (corresponding to the superelement modes) and physical coordinates (corresponding to the grid points on the superelement boundaries). CMS is advantageous because there are fewer modal coordinates than physical coordinates—perhaps only one percent as many. In addition, CMS can utilize modal test data, thereby increasing the accuracy of the overall analysis. 930 Structural Engineering Analysis and Design Second Edition 6.3.8 Modelling Flat Plates Using 2D Shells or 1D Grillages Grillage analyses may sometimes be used to model flat plates such as flat slabs. A grillage consists of 1D beams in two orthogonal directions to replicate the two-way spanning action that flat shells or plates perform perfectly. Two types of models may be used in both 1D grillages and 2D shells, i.e. with torsional stiffness or without. If torsional stiffness is specified, then it must be designed for. For the shell, the correct shear modulus G according to linear elastic theory G = E/(2(1+ν)) should model the torsional stiffness and thus must be designed for. To not have to design for the torsion, the shear modulus G should be manually set very low, although this makes the assumption that there is no shear flexibility modeled. This is because the shear rigidity is given approximately by GAs i.e. a function of the shear modulus as well. Now for grillages to replicate shells or plates, firstly since beams are used in two orthogonal directions, the density of the beams must be halved in order not to double up; Secondly, the bending rigidity D for a plate in theory should be EI/(1-ν2) instead of EI as for a rectangular beam. Thirdly, if torsion is to be designed for, the torsional rigidity GJ should be such that it is equal to the bending rigidity EI so that there is equal bending stiffness of the plate about any horizontal axis. Since G = E/(2(1+ν)), J should be set such that J = EI/G = 2I(1+ν). One of the advantages of using grillages instead of shells is the ability to design out torsional effects, i.e. by putting J = 0, shear deformations are still accounted for since G is still defined. 6.3.9 Modelling Down-Stand Beams on Structural Floors, Pile Caps and Changes in Thickness of Plates Floor slabs with down-stand beams, pile caps or changes in thickness of the plate should be modeled with offsets to the neutral axis of the local section. Down-stand beams should be modeled with offsets from the shells elements to the centroid of the down-stand beam, which is modeled as beam elements, NOT shells. Pile caps or local changes in thickness of a plate can be modeled with local shells offset (to their neutral axis) from the general plate elevation. Connections between elements should be at their neutral axis. Connections of slabs with offset beams are no different, the elastic neutral axis should be found and both the beams and the slabs should be offset from their common neutral axis to connect into column (beam) elements. This is important especially so in linear dynamic problems where an incorrect connection point will result in incorrect mode shapes. To model the offset in MSC.NASTRAN, three methods can be used. RBE2 or RBAR, both with ALL 6 DOFs of the single dependent grid constrained to ALL 6 DOFs of the single independent grid, repeated over each and every offset grid pair can be used. Alternatively this can be automated easily using ZOFFS on the shell element connection card, this being the recommended approach. Lastly, we could also use MID4, but this is not recommended. Note that offsets should be modeled because their would considerably increase the bending stiffness due to the Ar2 stiffness terms (by parallel axes theorem). Clearly both the bending stiffness and the membrane stiffness of the shell is required if offsets are modeled. 6.3.10 Modelling Stiffened Plates Modelling stiffeners using plate elements usually results in a too stiff representation. Stiffeners require cubic displacement functions to model the bending action, but shells in membrane action are capable of only linear or parabolic displacement interpolation. Hence, a single or two-shell element stiffener representation is almost always too stiff and peak stresses will be severely overestimated. Of course, with refinement, the model approaches the correct stiffness. The recommended approach is instead to use offset CBAR beam elements to model the stiffeners. 931 Structural Engineering Analysis and Design Second Edition 6.3.11 Modelling Connections Rigid joints do not allow relative rotation between connecting members whereas pinned joints do not transfer bending moments. Within the analysis code, a pinned ended beam element is akin to having a zero-length rigid link between the connecting members in all the DOFs except the rotational DOF that corresponds to the bending moment. This also means that we could theoretically model a partial fixity with a zero-length rotational spring between the rotational DOFs of the connecting elements. Modelling steel frames with pinned connections may sometimes be appropriate if we desire that all lateral loads are taken by the bracing members instead of through the moment connections. However, the rotations at pinned connection will be much greater, and the design must account for this. However, trusses are usually triangulated so that the lateral forces are accounted for by the inclined elements. Monolithic concrete frames are modeled with fixed connections. Connections in timber are usually pinned. RBE2 or RBAR elements can be used to define hinges or sliding joints. To model a hinge connection with an RBAR, use coincident grid points at the center of rotation and define an RBAR between the two grid points. This RBAR has zero length, which is acceptable for the RBAR. Make ALL 6 of the components associated with one grid point independent. Make only a select number of components of the other grid point dependent, leaving independent the components representing the hinge. With RBE2, again connect the two coincident nodes with an RBE2 with all DOFs of the dependent grid except that representing the hinge automatically dependent on ALL 6 DOFs of the independent grid. Both connections are then exactly the same. RBE2 is characteristic in the sense that ALL 6 DOFs of the independent grid is automatically selected, the user then has the option of selecting the DOFs of the dependent grid, but of more than one grid if intended. RBAR on the other hand, allows the option of selecting the DOFs of both the independent and dependent grid, but of only one pair. Modelling pinned connections in 2D and 3D elements require different considerations. Consider the modelling of a thin 2D lever with a pinned connection. The lever is allowed to pivot about a pin through its mounting hole. The interface between the lever and the pin is of consideration. Of course, to restrain all the nodes along the curve of the hole in translational and leaving the rotational DOFs free with respect to the basic coordinate system, is blatantly incorrect. To connect a ‘spider’ i.e. an RBE2 to all the dependent nodes on the curve of the hole and pin the independent node defined in the middle of the mounting hole may be acceptable, but this does (incorrectly) add stiffness to the model or rather an infinite rigidity around the hole (as if there was firstly, infinite friction between the curve lining the mounting hole and the pin, and secondly no allowance for the hole to expand radially or squash into an oval shape) as the constrained nodes cannot move in translation relative to each other, and hence the stress distribution around the hole will be totally incorrect. Another method to model this pinned connection would be to define independent SPCs around the outline curve of the hole, but ensuring that a local coordinate systems in cylindrical coordinates (a spherical coordinate system will be used in 3D problems requiring a pinned connection) is defined for all the constrained nodes. The nodes are of course constrained only in the radial direction to achieve the desired pivoting effect. Now each point on the curve of the hole is allowed to move tangentially and hence no stiffness or rigidity (or friction between curve lining the mounting hole and the pin) is added to the model and hence will produce the correct effect as the lever is allowed to pivot. But the stress distribution around the hole will still be inaccurate because the SPC would incorrectly resist the pull of the nodes away from the pin (hence not allowing the hole to expand) on top of correctly resisting the push. Hence, a manual iterative method must be undertaken to remove the SPCs that are resisting the pull of the lever away from the pin by inspecting the sign of the reaction on the SPCs. Gradually all the offending SPCs will be removed and the correct solution will be achieved. This similar effect can be attained automatically by modelling the pin explicitly and defining contact elements between the lever and the pin. This is probably the best method to model the pinned connection (be it in 2D or 3D). These contact elements can clearly resist the push but will not resist the separation between the lever and the pin. Of course, the orientation of these contact elements must be normal to the interface curves. 932 Structural Engineering Analysis and Design Second Edition 6.3.12 Modelling Spot Welds Spot welds are best modeled with CBUSH elements with large stiffness in all 6 DOFs in MSC.NASTRAN. Alternatively, RBAR or RBE2 (both with ALL 6 DOFs of the single dependent grid constrained to ALL 6DOFs of the single independent grid, repeated over each and every spot weld grid pair) elements may be used effectively. CELAS elements can also be used but is not recommended as apart from being extremely difficult to set up, problems with the generation of internal constraints may arise. The CWELD and PWELD entries are also ideal. Connections can now be established with ease between points, elements, patches, or any of their combinations. In short, the new CWELD connector element is general in purpose, easy to generate, less error-prone than any of the preceding methods, and always satisfies the condition of rigid body invariance. Test and analysis correlation has also been shown to be excellent. Connections can either be established conventionally, from point-to-point, or in a more advanced fashion between elements and/or patches of grid points. In the case of elements and patches, actual weld attachment points will usually occur within element domains or patches and will be computed automatically, with corresponding automatic creation of necessary grid points and degrees-of-freedom. Element- and patch-based connections, moreover, eliminate the need for congruent meshes. Reference grids that determine spot weld spacing, for example, can be defined beforehand which, when projected (using the CWELD entry) through the surfaces to be attached, uniquely determine the weld elements’ location and geometry. 6.3.13 Modelling Bolts CBAR elements can be used to model bolt element within a 2D or 3D mesh. Rigid elements can be used to model the finite dimension of the diameter of the bolt head or washer. Now if there is no tolerance between the bolt and its hole, then the bolt can be modeled with CROD elements to transfer only axial (and torsional) forces. 933 Structural Engineering Analysis and Design Second Edition 6.3.14 Modelling Applied Loads 6.3.14.1 Applied Concentrated Loads on One Dimensional Elements CBAR elements have cubic polynomial displacement functions, thus models linear variation in bending moment. Hence, point loads and moments should be only applied at the end nodes of the beam. A single structural beam member should be discretized by a number of CBAR elements to model the internal point loads. An internal point load results in a piecewise cubic variation of the transverse displacement, a mode of deformation that is not captured by the continuous cubic variation of the two-noded beam finite element. A continuous uniformly distributed load within a beam finite element results in a continuous quartic variation of the transverse displacement, again a mode of deformation that is not subsumed by the continuous cubic variation of the finite element. Applying internal loads onto beam elements will cause the equivalent nodal loads that the code computes based on the assumed interpolation function to be inaccurate. Hence the nodal displacements will in turn be inaccurate. On the other hand, if the loads are only applied at the nodes, we can be sure that the correct behavior is captured and thus there is no need for mesh refinement. 6.3.14.2 Applied Face and Line Loads on Two and Three Dimensional Elements Unlike beam elements, loads applied to shell elements should not be point loads or moments applied at the nodes. In theory, the stress under a point load is infinite and as the mesh is refined, the finite element method attempts to replicate the infinite stress. Consider a point load F at a single node with a characteristic element length ‘a’. As the model is refined, ‘a’ becomes smaller, and so the stress F/a becomes larger and tends toward infinity in the limit. This causes singularity. Now consider a pressure or distributed load P over n nodes. As the model is refined, the area of the pressure application stays the same, because it is related to the physical problem and not the mesh. While the number of nodes sharing in the pressure increases, the applied force at each node will decrease. The stress is equal to the pressure independently of the number of nodes, so there is no tendency towards infinity, and therefore no singularity. Singularities thus exist when a point load or likewise an SPC is applied to a shell or solid mesh simply due to the nature of a node having no area in the FEM. Even a needle tip, when observed under a microscope shows a finite tip radius. A point load in FEA on the other hand is applied on a node with no area. Hence the stress within the adjacent element increases as the mesh is refined. The results will never converge as the mesh is refined, as the solution become mesh-dependent. This is bad enough in h-element analysis, more so in pelement model, where the code will attempt to converge in a futile attempt. Hence, it is best to distribute the point load over a line or area although the interpolation function cannot model the resulting deformations exactly. This is perfectly acceptable, as unlike 1D beams, meshes of 2D shells have to be refined. Note that face loads (applied as a stress) are dependent upon the geometry of the face of the shell and line edge loads (applied as a stress) are dependent upon the thickness and the edge dimension of the shell. The following table lists the load and boundary conditions that will and will not cause a singularity. Load or Constraint on Beam Shell Solid Point No Yes Yes Curve or edge No No Yes Surface or face N/A No No Face or line loads should never be applied manually as individual equivalent concentrated loads. That is to say, a face pressure load should not be decomposed by the user by multiplying by the area and dividing by the number of grids on the face and applying these average concentrated loads all the grids on the face. This is because the user’s equivalent loading WOULD NOT be comparable to the true consistent loading. The equivalent loads at the grid points computed from the element loads are known as consistent loads, and they are calculated by applying the principle of virtual work. {f } = − {∫ [N] {b} dΩ} Τ Ω The same shape function that is used in deriving the element stiffness is used for arriving at this load-and hence the word consistent load. They are a function of the element types and the applied loads. 934 Structural Engineering Analysis and Design Second Edition 6.3.14.3 Applied Concentrated Loads on Two and Three Dimensional Elements Rigid elements such as RBE2 (with ALL 6 DOFs of the many dependent grids constrained automatically to ALL 6 DOFs of the single independent grid where the load is applied) are usually used to distribute specified force or moment to be applied onto a 2D or 3D mesh. Clearly, the independent grid point must correspond in space to the point of application of the external load, i.e. the elastic neutral axis of the section. Alternatively the RBE3 element may be used. The RBE3 element is a powerful tool for distributing applied loads and mass in a model. Unlike the RBAR and RBE2, the RBE3 does not add additional stiffness to your structure (a 2D shell mesh of a hollow tube being applied with a force or moment using an RBE2 “spider” to constrain all the grids on the section to the independent grid at the neutral axis center adds stiffness to the hollow tube section). Forces and moments applied to reference points are distributed to a set of independent degrees of freedom based on the RBE3 geometry and local weight factors. Basically, the external force is applied on the reference grid REFGRID in the component DOF direction REFC. The default action of this element is to place the REFC degrees of freedom in the m-set denoted by the grids GMi and components CMi after the field “UM”. C1 is then ALL 3 translational component (rotational components only used in special circumstances) numbers of the first group of independent grids G1,1, G1,2, G1,3,G1,4 etc … where the load is to be transferred to. $ BULK DATA RBE3 EID REFGRID REFC WT1 C1 G1,1 G1,2 G1,3 WT2 C2 G2,1 G2,2 Etc… WT3 C3 G3,1 G3,2 Etc… WT4 C4 G4,1 G4,2 Etc… “UM” GM1 CM1 GM2 CM2 GM3 CM3 GM4 CM4 GM5 CM5 Etc… To define a “spider” to transfer the beam type forces onto a 2D shell or 3D solid mesh, the REFGRID should correspond to a grid defined at the elastic neutral axis (centroid of section), the REFC should correspond to the component direction where the forces act i.e. in general 123456, WT1 denotes the weighting factor of the first group i.e. 1.0 for equal weighting here, C1 as 123 denotes the all three translational components of the independent grids of the first group G1,i which are the grids around the section. Note that C1 should be 123 even if there is force in only one or two translational directions. This is a software requirement as with all R-type elements to avoid singularity, not an engineering requirement. C1 should generally NEVER have any rotational components 456. Here only one group has been defined. Different groups are only required for different weighting factor to distribute the force. This occurs in certain groups of grids are deemed to be of different stiffness to the other grids. If a group of grids is deemed to be less stiff and hence attracting less force than that to the other grids, it will be justifiable to use a lower weighting factor to distribute less force to those group of grids. 935 Structural Engineering Analysis and Design Second Edition 6.3.15 Modelling Support Conditions When supporting 2D shells, it is best to apply the support conditions on all the nodes along the edge including the mid-side nodes in order to obtain a smooth stress variation along the edge. There will be a smooth variation of the bending stresses along and perpendicular to the edge and the through-thickness shear stress variation along and perpendicular to the edge. No stress singularity is introduced if the support condition is applied along the line. Of course, analogous to an applied point load, A SINGLE SPC applied on a 2D or 3D mesh will result in a singularity because a finite force value is applied on a node which has no area, hence the stress which is the force/area is infinite. The following table lists the load and boundary conditions that will and will not cause a singularity. Load or Constraint on Point Curve or edge Surface or face Beam No No N/A Shell Yes No No Solid Yes Yes No However, if stress recovery at the regions of the stress singularity is not required, then St. Venant’s Principle, which states that stress and deflection far from an applied load or constraint can be represented by a statically equivalent loading scenario, can be invoked. One of the fortunate characteristics of the FEM is that local effect will most likely have little effect on the global behaviour. Support stiffness is sometimes incorporated in the form of a ground spring, this may for instance model piles or foundations of different relative stiffness. This is only done to model the differential settlement. If the relative stiffness of ALL the supports is the same, then there is no reason to model the support stiffnesses. A ground spring is simply a spring eventually totally constrained to a rigid support. Reducing the stiffness of a support spring will probably reduce the force going into that support constraint, but the load must be accounted for elsewhere, i.e. all the load must be eventually accounted for. The total reactions must balance the total applied loading (assuming no ill-conditioning effects). 936 Structural Engineering Analysis and Design Second Edition 6.3.16 Primary and Secondary Component in Dynamic Analysis Primary and Secondary Systems kp mp ks ms Idealization when ωs/ωp > 2.0 kp mp + ms Idealization when ωs/ωp < 0.5 kp mp ks Secondary components may have to be included into the dynamic model of the primary component if they have frequencies comparable to those of the primary component. It is not the mass or the stiffness of the secondary component in isolation that matters in deciding whether they are dynamically prominent, but their natural frequencies. If the resonant frequencies of the secondary component are greater (ωs/ωp > 2.0) than those of the primary model, then they can be modeled as added mass on the primary system. If the resonant frequencies of the secondary component are lower (ωs/ωp < 0.5) than those of the primary model, then they can be modeled as stiffness (which are grounded, hence no mass DOF) on the primary system. Otherwise, the secondary system must be included within the dynamic model of the primary system. 6.3.17 Modelling Rigid Body Motion An excellent method of evaluating whether the intended rigid body motion is correctly represented within the finite element model is to perform a SOL 103. Note that AUTOSPC may have to be set to the non default value of NO to avoid grid point singularities from being constrained. The eigenvalue analysis also cannot model local mechanisms (identified by a critical MAXRATIO). But the eigenvalue analysis can model global mechanisms, i.e. the rigid body motion. The correct stiffness properties, boundary conditions and rigid element DOF dependency can be adjusted until the correct rigid body motions (at zero or close to zero frequencies) are obtained from visual inspection of the eigenvectors following an eigenvalue SOL 103 analysis. 937 Structural Engineering Analysis and Design Second Edition 6.3.18 Meshing Strategies With mesh refinement, the results will converge to the true solution for displacements and stresses. Stress analysis requires a much finer mesh density than static displacement response. This is because of the rate of convergence of displacement response being much greater than that of the stress. It would thus help to allow for fine discretization in regions of high stress gradient and stress concentrations such as: (a) near entrant corners, or sharply curved edges – using chordal deviation automatic meshing techniques say (b) in the vicinity of concentrated loads, concentrated reactions, cracks and cutouts (c) in the interior of structures with abrupt changes in thickness, material properties or cross sectional areas For 1D meshing, linear1D (1D elements from one 2D plane to another) or the linemesh automesher (line mesh along a line) can be used. For 2D meshing, uniform well shaped quadrilateral meshing is possible using spline and ruled within defined boundaries. It is also possible to extrude (along an arbitrary line) or to revolve a line to generate a 2D mesh. In the limit, the 2D automesher can be used to mesh irregularly any arbitrary planar surfaces with a combination of quads and triads. For 3D meshing, only volumes that can foreseeably be generated from extruding (in general along an arbitrary line) or revolving a planar 2D mesh can be meshed uniformly with the more accurate hexagonal elements. Meshing an enclosed volume of arbitrary shape often results in having to utilize the automesher (using either a fixed nominal element size or using chordal deviation techniques that refines the mesh size as the radius of curvature decreases), which employs tetrahedral meshes, hence a.k.a. tetramesher. CTETRA4 are constant strain elements and hence should be minimized since many more elements are required for convergence. The arbitrary volume can be better mapped with CTETRA10 elements utilizing the mid side node to model the surface curvature. Second order elements (QUAD8, TRIA6, TETRA10 and HEXA20) are useful in better approximating the curvature of the actual geometry due to their mid-side nodes. Hence it may be better to generate the mesh with second order elements straight away than to mesh with first order elements and only then change to second order elements. Automeshers are generally tetrameshers. Hexagonal automeshers are rare if not nonexistent, although a fair estimate would be that one would need 5 tetrahedrons for every brick element. Employing the automesher requires a clean geometry. For transferring geometry, kernel based geometry formats such as ACIS and Parasolids are recommended. Standard based geometry formats such as IGES, DXF and VDA may lead to translation errors. Inheriting a CAD geometry model often requires a cleanup operation to yield geometry suitable for the automesher. This process is certainly worth embarking upon before employing the automesher. One aspect of the geometry that must be cleaned up is short edges and sliver surfaces. Short edges occur in geometry when lines or surfaces do not meet exactly at the same point due to misalignment of features. Sliver surfaces (i.e. geometry surfaces with high aspect ratio) occur in geometry due to misalignment of features or due to the close proximity of fillet edges to other edges. Short edges and sliver surfaces with a dimension short compared to either the model size, or more importantly the nominal mesh size, will introduce errors into the model by forcing one edge of a triangle or quadrilateral to the length of that short dimension. This occurs because the automesher will try to space nodes on the geometry edges first and then within the geometry surfaces at the defined nominal element size. Since most automeshers are constrained to use every node and edge of the model, when short edges or short dimensions are encountered, a side of an element will be placed on the short edge whilst the other sides of the element will be of the user defined nominal element size. This clearly causes highly distorted elements. Limiting the size of the short edges to no less than 1/3 of the nominal element size is good practice. In short, the geometry should be checked for both short edges and sliver surfaces. The former is identified by checking for any short edge that may exist in the geometry due to the misalignment of lines or surfaces edges that should meet at a common point or common line, respectively. The latter is identified by firstly, checking for surfaces with high aspect ratio due to short edges which in turn is due to the misalignment of lines or surfaces that should meet at a common point or common line, respectively and secondly, by identifying lines or surface edges of close proximity belonging to different features. 938 Structural Engineering Analysis and Design Second Edition 6.3.19 Mesh Transition Techniques 6.3.19.1 Connecting 1D Elements to 2D Elements When connecting 2D shells to beams in the same plane, it is best to connect the beam to the mid-side nodes of the shells as well to ensure compatibility between the elements. Offsets should be modeled as this affects the stiffness greatly. No stress singularity is introduced as the beams are connected to all nodes lining an edge of shell elements within or on the edge of the shell mesh. When connecting one dimensional beam elements to shells orthogonally, special considerations must be observed. 2D shells are often used to model irregular flat slabs with 1D beams modelling the vertical columns. Very often we incorrectly model vertical columns fixed into a horizontal mesh of 2D shells at a particular node and perform stress recovery at the intersection. Obviously, as a 2D mesh is refined, theoretically, the stress (be it the bending or the shear) at the point of intersection goes to infinity (stress singularity), and the 2D mesh attempts to replicate that. However, since stress recovery (bending moment) at the pile tops are usually of concern in design for hogging, to read those values would be very much dependent upon the mesh size (mesh-dependent) and would simply be meaningless. Infinite stresses will result irrespective of the stress recovery procedure used in the shells, whether BILINEAR, CUBIC etc. Incidentally, if the mesh is not so fine, one can obtain pretty believable (but incorrect) answers, as the regions of stress concentration have not been reached. But it is when you refine the mesh that you suddenly start to get huge variations of stress (hence derived moment) and great discontinuities. To think that people normally associate 2D elements to give you more accurate results. One method is to use rigid RBE2s connecting the beam to a few nodes on the shell mesh in order to distribute the point load. The area over which the point load is distributed should replicate reality. The rigid connection should connect to all the nodes on the 2D element mesh within the relevant vicinity, i.e. including also the mid-side nodes. There will be no stress singularity. Another method is to mesh the pile tops of slab with beams with the same stiffness in line with methods of grillage analysis. Alternatively, a rigid may be incorporated with a dimension of the pile diameter to model the pile top, which is much stiffer and does not in reality act like a beam since it is very much constrained by the pile. These methods would be akin to moving the mesh transition region (here between two different elements in 1D beams and 2D shells) from the vicinity of interest (for stress recovery). But stress singularity still exists at the transition. Similar considerations apply when stress recovery is intended on the slabs over the edges supported monolithically by edge piles, which transfer moments. Again the edges of the slab can be meshed with beams in line with the methods of grillage analysis. But stress singularity still exists at the transition. Alternatively, since the slab is in series with the piles, the moment experienced at the edges of the slab must be equivalent to the moment in the piles. Hence the moment in the piles can be used to design for the moment in the edges of the slab. 939 Structural Engineering Analysis and Design Second Edition 6.3.19.2 Connecting 2D Elements to 3D Elements Solid elements have stiffness only in the translational DOFs at the attachment grid points; they have no stiffness for rotational DOFs. To connect a shell into a 3D mesh requires special modelling to connect the rotational DOFs of the shell into the 3D solid mesh. One method would be to add an additional layer of shells that continue into the solid mesh. Another method would be to use RBE2s (each RBE2 with ALL 6 DOFs of the many dependent grids on the solid mesh constrained automatically to ALL 6 DOFs of the single independent grid on the shell mesh) to rigidly connect the translational and rotational stiffnesses of the shell mesh to the translational stiffnesses of the solid mesh, although this will locally increase the model stiffness. RBE3s can be used to model the connection between shells and solids. By using RBE3s, the rotations of the attached grid points are simply slaved to the translations of the adjacent grid points. In the following example, two RBE3 cards are required. These RBE3 elements transmit the loads to the independent DOFs. If RBE2 elements are used, then the connection is “rigid.” $ BULK DATA $ RBE3 EID REFGRID REFC WT1 C1 G1,1 G1,2 RBE3 1 1 456 1.0 123 2 3 2 456 1.0 123 1 3 4 RBE3 2 4 An alternate method is to use the RSSCON element. When using the RSSCON capability, the shell element mesh must line up with the solid element mesh so that there is an exact element-to-element correspondence. RSSCON generates a multipoint constraint, which puts the shell degrees of freedom in the dependent set (m-set). The three translational degrees of freedom and the two rotational degrees of freedom of the shell edge are connected to the three translational degrees of freedom of the upper and lower solid edge. Poisson’s ratio effects and temperature loads are modeled correctly. There are two options for making this connection using the RSSCON entry, namely 1. The ELEM option, which allows you to specify the element ID of the shell and the element ID of the solid to which the shell is to be connected. 2. The GRID option, which allows you to specify the grid point ID of the shell and the upper and lower grid point IDs of the solid. Two triplets of grid point IDs may be specified on one RSSCON entry. 940 Structural Engineering Analysis and Design Second Edition The best modelling practice is when the height of the connected solid element is chosen equal to the thickness of the shell. If the height of the connected solid element is much larger than the thickness of the shell element, then the connection modeled with RSSCON will be stiffer than the continuum model. In a mesh where shell grid points are identical or coincide with solid grid points, the RSSCON Bulk Data entry may model a connection that is too stiff Connecting a shell into solid by extending the shell one layer into the solid WILL introduce stress concentrations. The best method would thus be to use rigids or RSSCON to connect transverse to plane of shell. Best Modelling Too Stiff Connections Other versatile connections are presented. The RSSCON connector produces excellent results if the user follows good modelling practices. The geometry of the RSSCON connector is checked, and fatal messages are issued for invalid connections. Additional recommendations are given below. 1. Midside noded elements should only be connected to other midside noded elements. For example, a CQUAD8 element connected to a CHEXA20 element is acceptable; however, a CQUAD4 element connected to a PENTA15 element is not allowed. Elements with missing midside grid points are not allowed. 2. For midside noded elements, avoid using the RSSCON where shells connect to triangular solid faces. 3. Do not mix coordinate systems when using midside nodes. In other words, when using midside nodes, do not define a local coordinate system containing all the shell grid points and the basic coordinate system to define the solid grid points. Otherwise, incorrect answers will be generated. 4. Only one edge of a single shell element may connect to a solid surface. 5. Do not connect more than one shell element to one solid element when using the ELEM option. 6. Do not attempt solid-shell connections to severely warped (greater than 20%) mid-side noded solid elements. 7. The plane of the shell element should not be parallel to the plane of the connecting face of the solid element. 8. The connecting edge of the shell element must lie in the face of the solid element. In addition, the vertex grid points of the shell edge connecting to a quadrilateral solid face must line up with its opposite edges; for triangular solid faces, the connections may be made between any of the edges. 941 Structural Engineering Analysis and Design Second Edition 6.3.19.3 Connecting 1D Elements to 3D Elements A method would be to use RBE2s to rigidly connect the translational and rotational stiffnesses of the beam to the translational stiffnesses of the solid mesh, although this will locally increase the model stiffness. Alternatively, one RBE3 element can make the connection. These RBE3 elements transmit the loads to the independent DOFs. If RBE2 elements are used, then the connection is “rigid.” $ BULK DATA $ RBE3 EID REFGRID REFC WT1 C1 G1,1 G1,2 RBE3 1 12 456 1.0 123 11 13 22 6.3.19.4 Fine to Coarse Mesh Transitions in Shell Meshes Compatibility would be satisfied across inter-element boundaries barring poor user meshing. For compatibility, the displacement function must be continuous across element boundaries, i.e. at least C0 continuity at these boundaries. Inter-element C0 continuity is satisfied for standard TRIA3, TRIA6, QUAD4, QUAD8, HEX8 and HEX20 elements. Compatibility is not satisfied when a QUAD4 is connected to the mid-side nodes of a QUAD8 or a TRIA3 to the mid-side nodes of a QUAD8 and other poorly formed connections or mesh transitions. Note however that QUAD8 connected to a TRIA6 will ensure compatibility. A good mesh transition for refinement is simply to use QUADs (instead of TRIAs) throughout the transition. QUAD mesh transition 942 Structural Engineering Analysis and Design Second Edition 6.3.20 Stress Singularity (Artificial Stress Concentration) and St. Venant’s Principle in Linear and Nonlinear (Material) Analysis Stress singularities exist when a single point load or a single SPC is applied on a shell or solid mesh. They also exist when a line of point loads or SPCs are employed on a solid mesh. The following table summarizes these conditions. Load or Constraint on Point Curve or edge Surface or face Beam No No N/A Shell Yes No No Solid Yes Yes No In perfect analogy, stress singularities also exist when a single beam element connects to a shell mesh. In all these cases, the stress singularity causes meaningless results as the mesh is refined as the ultimate solution becomes mesh dependent. Hence, they also cause p-element solution algorithms to fail as the code attempts, in vain, to converge to a finite solution. There are no stress singularity problems when shells are connected in plane, except at an internal corner in a planer shell mesh with zero radius subject to a membrane force where there will be an infinite stress if made from a perfectly elastic material. Generally, a radius must be created in the corner to achieve a measurable stress. The confusing issue with modelling this in finite elements is that sensible stresses can be predicted in the corner. This is just coincidence however; refinement of the mesh would see the stresses in the corner increase without limit. Internal corners should always be considered in any analysis as a potential failure area and these must have a realistic fillet radius inserted for convergent stress values to be predicted. Remember that the stress value reported in a non-filleted internal corner is only dependant on the element size and has nothing to do with any real value that might occur there. There is no stress singularity problems when shells are connected out of plane, except when a plane shell mesh subject to a membrane force is stiffened by another shell mesh oriented perpendicular to it in the direction of the membrane force. All these stress singularities can be avoided using proper modelling techniques. Single point loads should not be applied to a shell mesh, instead only edge loads or pressure loads. A single point load or a line of point loads should not be applied on a solid mesh, instead only pressure loads should be used. Note that equivalent user defined multiple point loads to represent edge loads (for shells) or pressure loads (for shells or solids) should not be attempted as the equivalent nodal loads generated depend on the shape functions of the particular element. {f } = − {∫Ω [ N]Τ {b} dΩ} Likewise, a single SPC should not be applied to a shell mesh, instead only a line or a surface patch of SPCs, and in both cases, SPCs should be applied also on the mid-side nodes of the elements if they exist. A single SPC or a line of SPCs should not be applied on a solid mesh, instead only a patch of SPCs, but also applying SPCs on the midside nodes of the elements if they exist. In perfect analogy, when 1D elements connect to 2D or 3D elements, multiple 1D elements should be used to avoid the stress singularity. For instance multiple gap elements to model the contact interface between two shell or solid meshes are perfectly acceptable. No stress singularity results. Likewise, no stress singularity exists when a beam mesh lines the edge of a group of shell elements within or at the edge of a shell mesh. The connection should however be compatible. Connecting the mid-side nodes if exist is recommended. Likewise, connecting a 2D shell mesh into a 3D solid mesh by extending the shell one layer into the solid WILL introduce stress concentrations. The best method would thus be to use rigids or RSSCON to connect transverse to 943 Structural Engineering Analysis and Design Second Edition plane of shell so that the membrane force is distributed, whilst still coupling the rotational DOF of the shell into the solid through their translational DOFs. However, if stress recovery at the regions of the stress singularity is not required, then St. Venant’s Principle, which states that stress and deflection far from an applied load or constraint can be represented by a statically equivalent loading scenario, can be invoked. One of the fortunate characteristics of the FEM is that local effect will most likely have little effect on the global behaviour. The above St. Venant principle is acceptable for linear analysis (on h-element analysis bur not linear adaptive p-element techniques). However, nonlinear material analysis will suffer from a similar problem as the adaptive p-element linear solution. High local stresses result from high local strains. A nonlinear material analysis will try to resolve the stiffness at a singularity by adjusting the material modulus as defined by its stress-strain relationship. Fictitiously high strains may cause additional nonlinear iterations that should not have been required by the true strain state of the model. Hence stress singularities must be avoided at all costs in nonlinear analyses. 944 Structural Engineering Analysis and Design Second Edition 6.3.21 Modelling Preload (Prestress) Preloads or prestresses are applied to elements such as cables and bolted joints to incorporate the differential stiffness within the calculations. Of course, the preload is also considered when performing stress recovery. A minimum of 2 runs is required to be able to simulate the correct preload in a bolted joint, but only if there is to be external loads applied to the system. If no external loads are to be applied, in say the simulation of bolt tightening, then the analysis can be executed in one run, even for a materially nonlinear response, as long as you accept the small displacement (geometrically linear) limitations of the method used. The preload applied to a bolted joint will cause the bolt to stretch and the clamped component (called the abutment) to be compressed. How much the bolt stretches and the abutment compresses depends on the relative stiffness of these two components. There are 3 methods for configuring the preload in MSC.NASTRAN, all with accompanying restrictions. These are the temperature load method, the MPC constraint method and the GAP element method. 6.3.21.1 Temperature Load Method This is the most general method and the only one that allows correct solution of a geometric nonlinear response. In this method, a negative temperature "freezes" the bolt so it contracts. Obtaining the correct preload in linear analysis requires 2 runs because you don't know the relative stiffnesses of the bolt and abutment. So you run once with any negative value of temperature and look at how much the bolt stretched and how much preload it induced. Now simply factor the temperature that freezes the bolt and re-run to obtain the correct preload. If the analysis is nonlinear, and the bolt or abutment will change stiffness due to deformation, this method becomes tiresome because you will need to iterate to find the correct preload as you try to follow the nonlinear force-displacement curve of the bolted joint. In this case, it is better to use the MPC method described below to obtain the approximate displacement of the bolt due to the preload. Of course, this will be limited by small displacement theory. Then you can apply the temperature to obtain the displacement from this run. This method also presents problems when real thermal loads are applied. Care must be taken to calculate a modified temperature for the bolt, which is now heated or frozen for 2 reasons. If external loads are to be applied, apply them as usual. 6.3.21.2 MPC Constraint Method MPC constraints in MSC.NASTRAN are subject to small displacement theory because the constraint direction is not updated due to deformation of the structure. Consequently, if the analysis is geometrically nonlinear, then the results may be inaccurate if the bolt direction changes significantly during analysis. Using beam elements with this method requires that the bolt is split somewhere along its length and the two parts of the bolt connected together with an RBE2 element in all directions except the axial direction. The axial direction of the two parts of the bolt is connected with an MPC and a third point (an SPOINT) is used to apply the preload (using an SLOAD entry). The displacement in the SPOINT from this run is recovered and used in a second run as the SPCD value to apply to the MPC (the SLOAD is removed for this run). Alternatively, you can now use this displacement to calculate the temperature to apply in a run similar to the one above. If external loads are to be applied, apply them as usual. 6.3.21.3 GAP Element Method The GAP element is subject to the same small displacement theory as MPCs, except the axial direction may have large displacement; large rotations are not supported. Again using beam elements with this method requires that the bolt is split somewhere along its length and the two parts of the bolt connected together with an RBE2 element in all directions except the axial direction. The axial direction of the two parts of the bolt is connected with a GAP element and the F0 field of the PGAP entry is used to specify the preload. Once again, the displacement (now in the GAP) from this run is recovered and used in a second run as the U0 value on the PGAP entry (F0 is left blank for this run). If external loads are to be applied, apply them as usual. In the MPC and GAP cases, if you use SLOAD or F0 respectively to load the bolted joint, this will give the correct behaviour as long as external loads are not applied. Applying external loads without using SPCD or U0 causes the load in the bolt not to change when the external load is applied; so 2 runs are needed to yield correct behaviour, but only when external loads are applied. 945 Structural Engineering Analysis and Design Second Edition 6.3.22 Modelling Symmetry A structure that has one or two planes of symmetry (irrespective of loading) can be half or quarter modeled, respectively. If the loads applied to the structure are symmetric relative to the plane of symmetry, then the full model can be replaced with half the model by applying a symmetric boundary condition. On the other hand, if the loads are antisymmetric, the same simplification can be achieved by applying the antisymmetric boundary condition. A symmetric boundary condition implies that the displacements normal to the plane of symmetry and rotations about the axes in the plane of symmetry are zero at the plane of symmetry. An antisymmetric boundary condition implies that the displacements in the plane of symmetry and rotations normal to the plane of symmetry are zero at the plane of symmetry. Even when the loading is not symmetric or antisymmetric about the structure’s plane of symmetry, advantage can be taken of symmetry. This is because any general loading pattern can be broken up into a combination of symmetric and antisymmetric loads relative to the plane of symmetry. SUBCASE 1 LABEL = SYMMETRIC CONSTRAINTS-Y LOAD SPC = 1 LOAD = 2 SUBCASE 2 LABEL = ANTISYMMETRIC CONSTRAINTS-Y LOAD SPC = 2 LOAD = 2 SUBCOM 3 LABEL = LEFT SIDE OF MODEL-Y LOAD SUBSEQ 1.0, 1.0 DISP=ALL SUBCOM 4 LABEL = RIGHT SIDE OF MODEL-Y LOAD SUBSEQ 1.0, -1.0 DISP=ALL The structure above can be analyzed with the half model but with 4 subcases. The first and second subcases model the symmetric and antisymmetric boundary conditions respectively, performing the analysis on the left half of the model. The third subcase combines the first and second subcases for the total results of the left half of the model. Finally, the fourth subcase computes the results of the right half of the structure. Symmetry modelling techniques are not recommended in modal and subsequent dynamic response analysis. Whilst a combination of symmetry and anti-symmetry can be used to find all the mode shapes, this combination is not feasible for most dynamic studies. Also avoid symmetry in buckling analysis. Symmetry is however a great idea in nonlinear static analyses. To apply symmetry conditions on a plane in a 3D model, all that is required is a set of translations SPCs in a direction normal to the cut plane. This would avoid Poisson effects at the boundary since contraction is not constrained in the plane of the cut, a scenario which will exist if all the nodes on the symmetry plane were connected by a rigid element (RBE2 with all 6 DOFs constrained) to an independent node on the neutral axis on which the 1D beam-like symmetry boundary conditions are applied. Symmetry conditions is different in elements that use mathematical representation (or DOFs) for their missing spatial dimensions, such as shell and beam models, where on top of the translation normal to the cut plane, the rotation about the two axes in the plane of the cut must be constrained. 946 Structural Engineering Analysis and Design Second Edition 6.3.23 Multi-Point Constraints (MPC) 21 Single-point constraints refer to zero and non-zero essential boundary conditions being applied to a particular node onto one or more of its DOFs. Single-point constraints with zero prescribed displacements are implemented by reducing the global stiffness matrix to a reduced stiffness matrix that does not include the equations pertaining to the constrained DOFs. In other words, within the static equilibrium equation [K]{U}={P}, the rows and columns (hence also the associated DOFs in {U}) of [K] and the rows of {P} associated with the constrained DOFs are eliminated. For non-zero prescribed displacements essential boundary conditions, the rows of [K] and {P} associated with the non-zero constrained DOFs are eliminated and the prescribed values of the constrained DOFs are included within the {U} vector. Of course, in a computer implementation, the global assembly procedure and the reduction process will be intertwined for efficiency. Multi-point constraints refer to constraints on multiple nodes. Three general methods of implementing multi-point constraints are: A. Master-Slave Elimination Using Rigid Elements with Case Control Command RIGID = LINEAR. The degrees of freedom involved in each MFC are separated into master and slave freedoms. The slave freedoms are then explicitly eliminated. The modified equations do not contain the slave freedoms. B. Penalty Augmentation Using CGAP Elements. Also called the penalty function method. Each MFC is viewed as the presence of a fictitious elastic structural element called penalty element that enforces it approximately. This element is parametrized by a numerical weight, w on the stiffness. The exact constraint is recovered if the weight, w goes to infinity. In other words, we are simply adding an appropriately stiff element between the constrained DOFs in order to simulate a constrained connection. The MFCs are imposed by augmenting the finite element model with the penalty elements. The theory behind using this method to simulate general non-zero constraints is described within Courant penalty functions. C. Lagrange Multiplier Adjunction Using Rigid Elements with Case Control Command RIGID = LAGR (also RIGID = LGELIM). For each MFC an additional unknown is adjoined to the master stiffness equations. Physically this set of unknowns represent constraint forces that would enforce the constraints exactly should there be applied to the unconstrained system. The master-slave elimination method is clearly the exact method of implementing multi-point constraints. However, the algorithm requires that dependent (slave) DOFs not be dependent upon more than one master DOF. The method also requires rearranging the equilibrium equations and hence is more computationally intensive. Nonlinear constraints are even more difficult to implement. The penalty function method on the other hand, adds an appropriately stiff element between the DOFs in order to simulate the correct prescribed displacement between them. For a zero displacement constraint, such as a rigid link, we would want the stiffness of the element to be as high as numerically possible. But unfortunately, the higher the ratio of the stiffness of the rigid link to the structure elements the more ill-conditioned the stiffness matrix will be. Obviously we have two effects at odds with each other. Making w larger reduces the constraint violation error but increases the solution error. The best w is that which makes both errors roughly equal in absolute value. This tradeoff value is difficult to find aside of systematically running numerical experiments. In practice the heuristic square root rule is often followed. This rule can be stated as follows. Suppose that the largest stiffness coefficient, before adding penalty elements, is of the order of 10k and that the working machine precision is p digits. Then choose penalty weights to be of order 10k+p/2 with the proviso that such a choice would not cause arithmetic overflow. The name “square root” arises because the recommended w is in fact 10k(10p)1/2. Thus it is seen that the choice of penalty weight by this rule involves knowledge of both stiffness magnitudes and floating-point hardware properties of the computer used. The penalty function method is less computationally intensive. There is no master21 FELIPPA, Carlos A. Introduction to Finite Element Methods. University of Colorado, 2001. 947 Structural Engineering Analysis and Design Second Edition slave interdependence and hence there is no restrictions on dependent DOFs unlike the master-slave elimination method. The penalty function method can also be readily used to implemented nonlinear constraints. The main disadvantage, however, is a serious one; the choice of weight values that balance solution accuracy with the violation of constraint conditions. For simple cases the square root rule mentioned previously often works, although effective use calls for knowledge of the magnitude of stiffness coefficients. Such knowledge may be difficult to extract from a general-purpose “black box” program. For complex cases selection of appropriate weights may require extensive numerical experimentation, wasting the user time with numerical games that have no bearing on the real objective, which is getting a solution. The deterioration of the condition number of the penalty-augmented stiffness matrix can have an even more serious side effect in some solution procedures such as eigenvalue extraction or iterative solvers. Finally, even if optimal weights are selected, the combined solution error cannot be lowered beyond a threshold value. The Lagrange Multiplier Adjunction method enforces the multi-point constraints by specifying appropriate forces at the associated DOFs. Since there forces or Lagrange multipliers λ are unknown before the solution is made, they are appended to the vector of original unknowns {U} by the process called adjuntion. The modified stiffness matrix is thus called the (multiplier-augmented) bordered stiffness matrix. This is solved for all the unknowns including the multiplier. In contrast to the penalty method, the method of Lagrange multipliers has the advantage of being exact (aside from computation errors). It provides directly the constraint forces, which are of interest in many applications. It does not require any guesses as regards weights. As the penalty method, it can be extended without difficulty to nonlinear constraints. It is not free of disadvantages. It introduces additional unknowns, requiring expansion of the original stiffness method. It renders the augmented stiffness matrix indefinite (i.e. no longer positive definite), a property that may cause grief with some solution methods such as Cholesky factorization or conjugate gradients. Finally, as the master-slave method, it is sensitive to the degree of linear independence of the constraints i.e. a DOF cannot be dependent upon more than one independent DOF. On the whole the Lagrangian multiplier method appear to be the most elegant for a general-purpose finite element program that is supposed to work as a “black box” by minimizing guesses and choices from its users. Its implementation, however, is not simple. Special care must be exercised to detect singularities due to constraint dependency and to account for the effect of loss of positive definiteness of the bordered stiffness on equation solvers. Generality Ease of implementation Sensitivity to user decisions Accuracy Sensitivity as regards to constraint dependence Retains positive definiteness Modification of DOF vector required Master-Slave Elimination Fair Poor to fair High Variable Penalty Function Excellent Good High Mediocre Lagrange Multiplier Excellent Fair Slight Excellent High None High Yes Yes Yes No No Yes 948 Structural Engineering Analysis and Design Second Edition 6.3.24 Model Checkout 6.3.24.1 Grid Point Singularities (AUTOSPC, EPZERO, K6ROT, SNORM) 6.3.24.1.1 AUTOSPC and EPZERO Grid point singularity is identified by considering the stiffness at each single node (contrast with mechanism type singularity which considers stiffness at more than one grid point). Since NASTRAN is primarily an implicit code, there is a need to remove DOFs with low or zero stiffness to avoid the stiffness matrix from becoming singular. The stiffness (and mass for that matter) in every DOF on a grid is provided by elements. CELAS elements provide axial stiffness only. CROD elements provide axial and torsional stiffness, but not torsional inertia. CBAR elements provide axial, torsional, bending, and shear stiffnesses but do not provide torsional inertia. Shells provide stiffness in all DOFs except for in the in-plane rotational DOF. Solids provide stiffness in only the 3 translational DOFs. If a DOF of a grid is unconstrained or if there is no contribution of stiffness from any element, then it has no stiffness and hence is singular, in which case an SPC must be automatically added using AUTOSPC. AUTOSPC scans the stiffness of the 6 DOFs at each grid. The stiffness ratio is the ratio of stiffness in the weakest direction to that in the strongest direction, considering all possible directions rather than just the coordinate direction. Translational and rotational stiffnesses are considered separately. NASTRAN then compares the STIFFNESS RATIOS with a failure criterion, to decide whether the DOF is singular and an SPC should be applied. At each grid, a 3 x 3 partition of the stiffness matrix for each of the three translational and three rotational DOFs is solved as an eigenvalue problem to determine the principal stiffnesses. Each stiffness term is compared to the principal stiffness using the formula where Kii is the term in the i-th row and i-th column of the matrix and Kmax is the principal stiffness. If ε is less than the value of PARAM, EPZERO, the global direction nearest i is considered singular. The default value for EPZERO is 10–8, but this can be adjusted using EPZERO, although this should be changed with great care. The default AUTOSPC is YES is all solution schemes except for SOL 106 and SOL 129. PARAM, AUTOSPC, YES PARAM, EPZERO, < Value 1.0E-8 by default > In a CBAR assemblage with all the stiffness (axial, torsion, bending in 2 directions and optionally shear in 2 directions) properties specified, no AUTOSPC is required as there are 6 stiffness contributions to every DOF. In CBAR assemblage with missing stiffness properties or likewise in CROD assemblages, certain DOFs may have to be suppressed as there may be no stiffness contribution. In the limit, if a single DOF spring solitarily connects a node, all other DOFs of the node will be constrained except for the DOF in which the spring acts. Likewise, rotational DOFs of solids and in-plane rotational DOFs of shells are constrained. Solids have no rotational DOFs and shells do not have in plane rotational DOFs. This is because of the nature of shells providing in plane rotational stiffness through the in plane translational stiffnesses of many elements within the surface mesh and solids providing rotational stiffness about the three axes through the translational stiffnesses of many elements within the volume mesh. 949 Structural Engineering Analysis and Design Second Edition The DOFs constrained by the program must be checked, since over-constraining can cause incorrect results. The potentiality of over-constraining is usually associated with 1D elements. Constraining the in-plane rotational DOFs of shells and all 3 rotational DOFs of solids do not generally over-constrain the model as the rotational stiffnesses (and associated deformations) in 2D and 3D elements, by their very nature, are provided by the stiffness of the many translational DOFs. The potentiality of over-constraining a finite element model consisting of 1D elements shall be investigated thoroughly. To this end, it is crucial to know the nature of the load path in the structure being modeled. All applied loads must be balanced ultimately by the reactions through certain types of effects (which appear as internal forces and stresses) within the structure. There are 4 ways of carrying load, namely in axial force, in torsion, in bending moment and in shear force. These lead to deformations. An axial force causes axial deformation, torsion causes torsional deformation, bending moments cause bending deformations and shear forces cause shear deformations. If it is envisaged that a particular load path does not involve significant bending moment and shear force, that load path can be modeled with a CROD element. (Note that CBAR elements become CROD elements if both ends are pinned in bending rotations (not torsional) or if a very small value of bending stiffness is inputted such that the bending moment becomes very small. A pinned ended beam element is akin to having a zero-length rigid link between the connecting members in all the DOFs except the rotational DOF that corresponds to the bending moment). The main nature of the load path on outrigger columns on a sky-scrapper is in axial force. CROD elements may be sufficient in this case. The same argument applies for using CROD elements to model a truss where the load path is primarily axial in nature. However, CROD elements or pin-ended CBAR elements provide no rotational stiffness to the DOFs. To avoid a singular matrix, these DOFs are artificially constrained using AUTOSPC. The user must then ensure that these lost loads into these artificial constraints are small enough to be ignored. The applied loads are no longer totally balanced by the actual support reactions, but some energy is lost into the artificial constraints. If the load path is primarily axial, the loads lost into these artificial constraints will be small. But if a significant force is lost into the artificial constraint, the model is deemed to be overconstrained. The load path is not primarily axial in nature. CROD elements should hence not be used to model a load path where there are significant bending and shear actions as there will be no bending stiffness to transfer the loads. This will cause a mechanism (singular matrix) to occur unless an automatic constraint is placed by AUTOSPC. If however, CBAR elements are used with bending stiffness contribution in the outrigger and the truss examples, the potentiality of there being some bending action is accounted for, just in case. It will of course be observed that the bending moments and shear forces in the outriggers and the truss CBAR elements to be small if the load path is primarily axial in nature. No singularities exist when CBAR elements (with axial, torsion, bending and optionally shear stiffnesses) are used. Akin to the outrigger and truss examples, applying a concentrated moment on a cable in reality will result in a mechanism. That is to say, applying a concentrated moment about the common grid adjoining two collinear CROD elements will be futile, as the DOF will be constrained by AUTOSPC, as it has no stiffness to resist the moment. The moment load is lost into the constraint, again because the anticipated load path was not modeled by the element. If however, a CBAR element of very low stiffness is added to the grid, such that AUTOSPC does not constrain the DOF, the application of the concentrated moment will cause the displacements to be very large, as the resistance is very low. Likewise, torsional stiffness in CBAR elements can often be ignored if there is deemed to be little torsional forces i.e. that torsion is an insignificant load path. If a DOF has no torsional stiffness component, then the DOF component will be automatically constrained by the code. But if a torsion load path is intended, the torsion will be lost into the artificial constraint, making the structure incorrectly too stiff. If on the other hand, the stiffness in that DOF component is not too small in comparison with the other DOFs in that particular grid such that AUTOSPC is not invoked, the torsional forces will cause large torsional deformations within the element. To conclude, if a DOF is without stiffness and is not constrained by the user, then a grid point singularity will exist unless the code enforces an artificial restraint by AUTOSPC. If the DOF is part of a critical load path, then loads will be lost into the artificial constraint instead of being carried by the action of the structural elements and ultimately being transferred into the real supports. If instead the DOF has a low stiffness, but not low enough to be constrained by AUTOSPC, then the matrix will not be singular (although likely to be quite ill-conditioned depending on the precision of the machine), but the applied loads will cause a large deflection as the resistance is low. 950 Structural Engineering Analysis and Design Second Edition 6.3.24.1.2 K6ROT and SNORM For linear solutions (i.e. all except SOL 106 and SOL 129), the default K6ROT is 0.0, whilst for nonlinear analysis the default is 100.0 (this is opposite to the defaults for AUTOSPC). K6ROT is intended primarily for geometric nonlinear analysis. For highly nonlinear solutions a value of 1.E5 has been used successfully. NASTRAN internally inspects an appropriate rotational stiffness value to be applied, this value is then multiplied by K6ROT. For most instances, the default is appropriate. There may be instances where K6ROT is beneficial in linear analysis. Shell elements do not have stiffness in rotation about an axis normal to the shell. In models consisting of thousands of shell without reinforcement (e.g. car models) this can produce a very long list of singularities, making checking tedious. This may be solved with K6ROT, which removes the singularity (and prevents AUTOSPC) by specifying a small value of stiffness in the rotational degree of freedom. In other words, a grounded in-plane rotational spring is inserted to remove the singularity. Secondly, for linear analysis, if a surface is flat, then there is no reason why we cannot allow AUTOSPC to automatically constraint the in-plane rotational freedoms. If however, the surface is only slightly curved (say 179° between adjacent shell elements), then letting AUTOSPC constrain the freedoms may be unacceptable, as the model may not pass the rigid body checks (GROUNDCHECK). In this case, K6ROT with a value of 1.0 may be deemed appropriate. PARAM, K6ROT, < 0.0 to 100.0 > In linear analysis, instead of using K6ROT, it is better to use PARAM, SNORM. By default, the direction of the normal rotation vector for flat plate elements is assumed to be perpendicular to the plane of each element. If the model is curved, the shell bending and twist moments must change direction at the element intersection. If transverse shear flexibility is present, the deformations may be too large. (Because elements using low-order formulations ignore the edge effect, this rarely causes any problems-a large value of the parameter K6ROT partially cures the problem). With the unique normal (SNORM) option, the rotational degrees of freedom at each corner of an element are measured relative to the specified normal vector direction. Thus, all elements connected to a grid point will use a consistent direction for defining shell bending and twisting moments. Shell normals are available for CQUAD4, CQUADR, CTRIA3, and CTRIAR elements. Normals are activated if the actual angle between the local element normal and the unique grid point normal is less than 20.0°, the default value. The default can be changed by setting SNORM to the desired real value up to 89°. The unique grid point normal is the average of all local shell element normals at a specific grid point. Generated grid point normals may be overwritten by userdefined normals. A shell normal defines a unique direction for the rotational degrees of freedom of all adjacent elements. A shell normal vector is created by averaging the normal vectors of the attached elements. If the actual angle is greater than the value defined on PARAM, SNORM, (default = 20.0) the edge is assumed to be a corner, and the old method is used. Shell normals improve the accuracy of the results in curved shells where in-plane shear and twisting moments act together. The type of structure that exhibits the most change in results is a thick curved shell with large in-plane shear forces and twisting moments. Most other problems, such as flat plates and curved shells with pressure loads, show changes in results of less than 1%. More degrees of freedom may be constrained using this improved formulation. This formulation results in zero in-plane rotational stiffness values. The CQUAD8 and CTRIA6 elements are not included in the shell normal processing. If they are modeled correctly, they do not require shell normal processing. Connecting these elements to the lower-order flat elements is not recommended. Transverse shear flexibility (MID3 on the PSHELL property entry) should be left on when normals are used. PARAM, SNORM, 20.0 $ Default value is 20.0 In linear solutions, PARAM, K6ROT, 0.0 and PARAM, SNORM, 20.0 are recommended. Transverse shear flexibility (MID3 of PSHELL) should be included. AUTOSPC should also be switched on (as is the default in linear analysis). K6ROT can be used in linear analysis to reduce the output in the Grid Point Singularity Table due to AUTOSPC, simply for ease of checking the automatic constraint DOFs normally more critical for 1D elements. It can also be used with a value of 1.0 in linear analysis when the shell surface is only slightly curved. However, K6ROT with values of around 100.0 is intended primarily for nonlinear analysis. 951 Structural Engineering Analysis and Design Second Edition 6.3.24.2 Mechanism Singularity of Stiffness Matrix (MAXRATIO, BAILOUT) A mechanism type singularity requires the consideration of stiffness at more than one grid point (contrast with grid point singularity which considers stiffness at each grid). MAXRATIO checks for I. global mechanism singularity, and for II. local mechanisms singularity within the system. AUTOSPC may have accounted for all the local grid point singularities (of beam grids without certain stiffness properties, in plane rotational freedom of shell grids and all rotational freedoms of solid grids), but it remains to be seen if the system is restrained globally from rigid body motion or if there are local mechanisms. Mathematically, a mechanism type singularity is detected during decomposition, based on the maximum ratio of the matrix diagonal to the factor diagonal Log10 MAXRATIO indicates how many significant digits may have been lost during the decomposition. where Kii is the i-th diagonal term of the original stiffness matrix and Dii is the i-th diagonal term of the factor diagonal matrix. Note that for a symmetric matrix K it can be represented as If for any row i, this ratio is greater then MAXRATIO, then the matrix will be considered nearly singular (having mechanisms). If any diagonal terms of the factor are negative, the stiffness matrix will be implausible (non-positive definite). The exact grid point failing the criteria is not significant for the global rigid-body mechanisms and may change with small changes in the model; The exact grid point failing the criteria is significant for the local mechanism. NASTRAN then takes appropriate action depending on the BAILOUT parameter. If negative, NASTRAN is directed to continue processing. PARAM, BAILOUT should really therefore NOT BE USED (it should be specified 0 to terminate the analysis if near singularities are detected), instead of failing the MAXRATIO, the modelling should be corrected. $ BULK DATA PARAM, MAXRATIO, < Value 1.0E5 by default > PARAM, BAILOUT, < 0 or –1 > Should be positive and less than 1.0E5 First, consider the global mechanism. For a fully coupled structure, there can be 6 global rigid body motions, which must all be constrained. Non fully coupled portions of the structure exhibiting rigid body motion can also be regarded as a global mechanism. Translational rigid body motion can be constrained by the user applying the 3 DOF translational constraints at a particular grid or at multiple grids (of course not all 3 DOF constraints need to be applied at the very same grid, so long as the structure cannot exhibit rigid body translation on the whole). As for rotational rigid body motion, the manner in which constraints need to be applied to restrain the rigid body modes depend on the type of model, whether beams, shells or solids. Beam models can be completely restrained against rotational rigid body motion by applying the 3 rotational DOF constraints at any one grid. Shell models can be restrained against the 2 out-of-plane rotational rigid body motion by applying the 2 rotational DOF constraints at any one grid. However, the in plane rotational rigid body motion CANNOT BE constrained by applying a in-plane rotation restraint at a grid or multiple grids (as AUTOSPC does) because individual shell elements do not have any 952 Structural Engineering Analysis and Design Second Edition in-plane rotational stiffness in general. But of course, the shell mesh as a whole does have in plane rotational stiffness. Thus, the in plane rotational rigid body motion can only be suppressed by a set of translational DOFs in the two directions in the plane of the shells applied at different grids. Alternatively, a set of grids can be connected to a grid with an RBE2, which is then suppressed in its rotational freedoms. Likewise, with solid models, all 3 rotational rigid body motions CANNOT BE suppressed by applying rotational DOF constraints at a grid or multiple grids (as AUTOSPC does) because individual solid elements have not any rotational stiffness. But of course, the solid mesh as a whole does have rotational stiffnesses about the 3 axes. These are suppressed by a set of translational DOFs in the three directions applied at different grids. Alternatively, a set of grids can be connected to a grid with an RBE2, which is then suppressed in its rotational freedoms. On all three type of models, be it beam, shell or solid models, a set of translational DOF constraints in the 3 directions applied at different grids will act to constrain the rotational rigid body motion. It must be remembered of course, that these application of constraints will act to alter the behaviour of the model and hence should be representative of reality. Second, consider local mechanisms. Local mechanisms refer to individual finite elements. Local mechanisms occur when an element if not properly connected to the main structure. That is to say, its stiffnesses are not fully coupled into the main structure. It is best to illustrate with examples. A local mechanism will exist if a CBAR or CBEAM has no torsional stiffness whilst its adjacent collinear beams have torsional stiffness. The local beam may exhibit rigid body motion, as the torsional stiffness (and hence the ability to prevent the spinning about the axis) of the element is not attached onto the main structure. This would not be prevented by AUTOSPC because there is a stiffness contribution to the torsional DOF from the adjacent elements. A local mechanism also occurs when a CBAR or CBEAM is pinned in all three rotational DOFs on both ends, irrespective of whether it is collinear of not with adjacent beams. Note that to model trusses, only the two bending rotational DOFs are released, not the torsional DOF. This is perfectly acceptable. Likewise, pinned ended (in the two bending rotation DOFs) beams on multi-storey buildings can be used so long as the torsional DOF is not also released. But if the torsional stiffness was forgotten on either the truss or the multi-storey building, then the beam can spin about its axis. This also occurs when all 3 rotation DOFs of the two ends of the beam are released. The about-axis rotation motion of the beam is not connected onto the main structure and hence is a local mechanism. This would not be prevented by AUTOSPC because there are contributions to the rotational stiffness from adjacent elements, which are not pinned ended. Next, a local mechanism can occur if shells elements without bending properties (MID2 on PSHELL) are used. This however may be prevented by AUTOSPC. A local mechanism can also occur if a CBAR or CBEAM element connects into shells elements without special modelling techniques to transfer the in-plane (of the shell) moment. Hence if a 1D element connects to the surface of the shell mesh, there is no coupling of the in-plane rotational stiffness, and hence the 1D element is a mechanism as it can spin about the axis normal to the shell surface. This would not be prevented by AUTOSPC as the beam provides the rotational stiffness. An RBE2 or RBE3 connection should instead be employed. A local mechanism also occurs when a CBAR or CBEAM connects onto one grid of a solid mesh, even if the other end of the CBAR or CBEAM is also connected onto the solid mesh. Again there is nothing to stop the beam from spinning about its axis as the rotational motion is not coupled into the solid mesh. This would not be prevented by AUTOSPC as the beam provides the 3 rotational stiffnesses. An RBE2 or RBE3 connection should be employed. Next, a local mechanism occurs also when a shell mesh is connected into a solid mesh without proper modelling techniques to connect the out-of-plane (of the shell) rotational stiffnesses. This would not be prevented by AUTOSPC as the shell mesh provides the out-of-plane (of the shell) rotational stiffnesses. Global mechanisms are best pin-pointed by running a SOL 103 (with AUTOSPC possibly set to the nondefault value of NO) and visually inspecting the modes of vibration that have zero (or close to zero) frequency. This will highlight the global rigid body motion of the entire structure and also the non fully coupled portions of the structure as mechanisms. Local mechanisms on the other hand will cause a SOL 103 to crash and the DOFs with a critical MAXRATIO will be presented in the .f06 file for inspection and subsequent attention. 953 Structural Engineering Analysis and Design Second Edition 6.3.24.3 Grid Point Singularities (AUTOSPC, K6ROT) and Local and Global Mechanism Singularity (MAXRATIO, BAILOUT) for Linear, Nonlinear, Static and Dynamic Solutions Solution Grid Point Singularity Linear static SOL 101 Linear buckling SOL 105 AUTOSPC, YES K6ROT, 0.0. Nonlinear static SOL 106 AUTOSPC, NO K6ROT, 100.0 Linear modal SOL 103 AUTOSPC, YES K6ROT, 0.0. Linear dynamic SOL 109, AUTOSPC, YES SOL 112, SOL 108, SOL K6ROT, 0.0. 111 Nonlinear dynamic (implicit) SOL 129 AUTOSPC, NO K6ROT, 100.0. Nonlinear dynamic (explicit) LS-DYNA None Local and Global Mechanism Singularity Local mechanisms (identified with critical MAXRATIOs) may cause the solution scheme to crash, failing which the results would be suspect. Global mechanisms cannot be modeled, the structure must be at least statically determinate by applying sufficient zero or prescribed displacement boundary conditions. Local and global mechanisms show up as critical MAXRATIOs. Local mechanisms (identified with critical MAXRATIOs) may cause the solution scheme to diverge, failing which the results would be suspect. Global mechanisms (identified by a SOL 103 with AUTOSPC possibly NO) cannot be modeled because convergence to a static equilibrium state can never be achieved, hence all parts of the structure must be at least statically determinate by applying sufficient zero or prescribed displacement boundary conditions. Local mechanisms (identified with critical MAXRATIOs) may cause the solution scheme to crash, failing which the results would be suspect. Global mechanisms can be modeled (possibly with having to set AUTOSPC to the non-default value of NO), showing up as zero frequency modes. Intentional or unintentional global mechanisms can be readily visible, inspected and attended to. Local mechanisms (identified with critical MAXRATIOs) may cause the solution scheme to crash, failing which the results would be suspect. Global mechanisms can be modeled as long as the unrestrained degree of freedom has defined mass terms. Note that since the analysis is linear, the stiffness and damping is based on the initial undeflected geometry. Must eliminate unintentional global mechanisms, otherwise the mechanism will continue vibrating, possibly inducing incorrect results. Local mechanisms (identified with critical MAXRATIOs) may cause the solution scheme to diverge, failing which the results would be suspect. Global mechanisms can be modeled as long as the unrestrained degree of freedom has defined mass terms. Must eliminate unintentional global mechanisms, otherwise the mechanism will continue vibrating, possibly inducing incorrect results. Local mechanisms will introduce errors. Global mechanisms can be modeled as long as the unrestrained degree of freedom has defined mass terms. Must eliminate unintentional global mechanisms, otherwise the mechanism will continue vibrating, possibly inducing incorrect results. 954 Structural Engineering Analysis and Design Second Edition 6.3.24.4 Ill-Conditioning of Stiffness Matrix (EPSILON, Load and Reaction Discrepancy PRTRESLT) Singularities occur when there is no stiffness (or very low stiffness) in a DOF component relative to other DOF components at a particular node. The contribution of stiffness may come from any element. The relative contribution of the adjacent elements is immaterial. On the other hand, ill-conditioning occurs when the relative stiffness contribution in a particular DOF component at a node from adjacent elements is large. For illustration, take an example of two springs in series of stiffness k1 and k2. Assume k2 >> k1. k1 F k2 Two equations can be written for this 2-DOF system, namely (k1 + k2) u1 + (−k2) u2 = 0 (−k2) u1 + (k2) u2 = F which can be solved simultaneous for the two displacement unknowns. Getting rid of u2 from the two equations without performing any arithmetic, the displacement for u1 is obtained as u1 = F / (k1 + k2 − k2 ) Now if k2 >> k1 then there will be error e = k2 − k2 (not zero due to numerical inaccuracy) introduced in the calculation of u1. And because the value of the second k2 is large compared to k1, e would be comparable in magnitude to k1. Subsequently, the force in the first element will be calculated as f1 = k1 u1 = F k1 / (k1 + e) when in reality it should be f1 = k1 u1 = F Hence, ill-conditioning occurs when there is large differences in stiffness between adjacent DOF components at a particular grid point. A definite indication of ill-conditioning is when the sum of loading at a particular load due to explicit nodal loads and also equivalent element loads is not equal the sum of the element end forces for all the elements connected to that particular node. Codes generally perform an out-of-balance check to detect illconditioned matrices. In MSC.NASRAN, the condition of overall stiffness matrix is ascertained using EPSILON in the .f06 file. If all the stiffness terms in the matrix are of the same order of magnitude then the numerical calculations carried out NASTRAN on the matrix are easy. However, if there are very large differences between the largest and smallest stiffness terms then the accuracy of the analysis will be impaired due to limitations of computer numerical accuracy. The matrix is then considered to ill-conditioned. EPSILON is based on a strain energy error ratio. The EPSILON value should theoretically be equal to zero, but due to computer accuracy limitations it usually in the order of 10-7 to 10-8. Large values indicate that the stiffness matrix is ill-conditioned. A system of linear equations is said to be ill-conditioned if small perturbations in the system lead to large changes in the solution. NASTRAN checks for evidence of ill-conditioning in the system of equations representing the structural model. An EPSILON value of 1 would indicate that parts of the model are disconnected, or that there is a mechanism in the structure. Hence an EPSILON value of 1 would be obtained if the model fails the MAXRATIO check, i.e. the global singularity (rigid body motion) or local mechanism check. The upper limit for EPSILON is a matter of judgment. Usually, analyses producing EPSILON values below 10-9 are considered acceptable. A large value of epsilon (greater than about 10-3) is an indication of numerical illconditioning and requires further investigation. It does not matter whether epsilon is positive or negative, as long as it is small. In addition, a value of, say, 10-12 is not a "better" value than 10-10; both are "small enough". After decomposition, a singularity may lead to an incorrect solution. In static analysis, MSC.NASTRAN solves to obtain u (displacements). Using these displacements, a “residual” loading vector is calculated as follows: 955 Structural Engineering Analysis and Design Second Edition This residual vector should theoretically be null but may not be null due to numeric roundoff. To obtain a normalized value of the residual loading, an error measure EPSILON is calculated by Alternatively, ill-conditioning can be ascertained by inspecting the discrepancy between the applied forces and reactions. The following PRTRESLT parameter prints the resultant of the applied loads (OLOAD RESULTANTS), the resultant of the restraints (SPCFORCE RESULTANTS and MPCFORCE RESULTANTS) all about the point specified by PARAM, GRDPRT, N, the default being the origin of the basic coordinate system. $ BULK DATA PARAM, PRTRESLT, YES The EQUILIBRIUM Case Control Command can also be used to perform the equilibrium balance check. To conclude, ill-conditioning indicated by high values of EPSILON is caused by a high difference in stiffness between adjacent elements in the model (the solution of which would obviously be to use rigid elements such as RBE2 connecting the corresponding stiffness to model the much stiffer element) and by large mass in dynamic analysis whilst ill-conditioning indicated by an EPSILON value of 1.0 is caused when the model fails the MAXRATIO check, i.e. the global singularity (rigid body motion) or local mechanism check. 956 Structural Engineering Analysis and Design Second Edition 6.3.24.5 Grid Point Weight Generator The total mass and inertia of the model can be checked by specifying the GRDPNT, N parameter with respect to the grid point N, a value of N = 0 denoting the origin of the model coordinate frame being used. $ BULK DATA PARAM, GRDPNT, < 0 for about origin or specify a Grid ID > 6.3.24.6 Displacement Compatibility Check Displacement compatibility refers the fact that the displacement shape functions are continuous between adjacent elements. For instance, the corner and mod-side nodes of adjacent elements must be connected and so a mesh transition is required for a mesh of linear elements to mesh into parabolic elements. To ensure displacement compatibility between adjacent elements, a preprocessor should be used to perform a visual inspection on a shrink plot of all the elements from their nodes. Missing elements may be detected visually. More effectively, the pre-processor should be used to plot the free ends (1d mesh), free edges (2d mesh) and free faces (for 3D mesh) of the model. Unintentional holes and incompatibility within the model will clearly show up in the display. A real modal analysis (assuming mass correctly incorporated) can also be performed to ensure that all parts of the model are properly connected. Or, a 1g i.e. gravity load static analysis in the 3 directions (in 3 separate subcases) can be performed (assuming mass correctly incorporated) to check for displacement incompatibilities. To zip up the unconnected grids that are coincident (to a tolerance applicable to model), the equivalence function of the pre-processor may be used. However, ensure that intentional coincident grids that model scalar stiffness, scalar damping or hinges are not equivalenced. 957 Structural Engineering Analysis and Design Second Edition 6.3.24.7 Element Quality Checks It has been mentioned that the benefits of isoparametric element formulations is that curved geometries can be mapped more accurately because the geometry is also described by the shape functions. However, the geometry must not be too distorted, whether in its initial undeflected configuration or at a later stage of a nonlinear analysis. The parameter that suffers from badly distorted configurations is the Jacobian | J |. The Jacobian maps the natural coordinates to the global coordinates in the stiffness expression of the elements. Element distortions generally stem from excessive variations in the Jacobian between different nodes. Codes tend to (based on experience) place bounds on the permissible variation of the Jacobian over a particular element between different nodes. Re-entrant angles (where the corner node of a QUAD8 is squeezed into the element beyond the mid-point must be avoided as the will cause the Jacobian to change sign. As the corner node approaches the mid-point, | J | 0, causing infinite strains. Even in an undistorted QUAD8, if the mid-side node were beyond the middle third, this would cause the Jacobian to vanish at a certain node and hence again produce infinite strains. There are four possible forms of element distortion, namely: (i) Aspect ratio distortion (ii) Angular distortion, i.e. skew and taper (iii) Volumetric distortion (iv) Mid node position distortion All these distortions can be quantified as some terms in the Jacobian going to zero, causing a numerical singularity arising solely from the mapping function. It can lead to large errors in the stress results but has a lesser effect on the computed displacements. These numerical singularities have been used in elements modelling cracks. The default element quality checks in MSC.NASTRAN are presented as follows. If any of these are violated, then the analysis will crash. The following are the default MSC.NASTRAN element quality values which should be ensured within the pre-processor. A few of these default values can be changed using the GEOMCHECK Executive command. Evaluates location of mid-side nodes The results are printed under USER INFORMATION MESSAGE 7555. 958 Structural Engineering Analysis and Design Second Edition 6.3.24.8 Maximum Values The summary of maximum displacements, loads and SPCs and MPCs all in the basic coordinate system can be requested using the following parameter. $ BULK DATA PARAM, PRTMAXIM, YES Subcase Number 6.3.24.9 Element Orientation Check The element X-, Y- and Z- orientation for beams must be consistent as stress recovery is presented in the element coordinate system, the Z-normal for shells must be consistent but the element X- and Y- orientation can be random as long as the stress recovery is presented in the global coordinate system, and for solids a random X-, Yand Z- element orientation is fine as long as the stress recovery is presented in the global coordinate system. 6.3.24.10 Duplicate Grid and Element Check A pre-processor should be equipped with the ability to detect duplicate grids or elements, be it beams, shells or solids, as visual inspection is impossible. Unintentional duplicate grids occur when an equivalence operation was forgotten. Duplicate grids may however be intentional for the modelling of scalar elements CELAS, CBUSH or rigid elements RBE2. Duplicate elements may occur if a line, surface or volume was accidentally meshed more than once. 6.3.24.11 Element Summary Table The ELSUM Case Control command provides a quick summary table of properties for the elements in the model. These properties include element-id, material-id, length (or thickness), area, volume, structural mass, non-structural mass, total mass, and weight (weight mass * total mass). 959 Structural Engineering Analysis and Design Second Edition 6.3.24.12 Unconstrained Equilibrium Check (Grounding Check) 6.3.24.12.1 Enforced Displacement Method This is a superb method of evaluating some modelling errors that cause unintentional grounding of the structure. If a structure is truly unconstrained, then movement at one point of this structure should cause the whole structure to move as a rigid body. The following procedure can be used to perform this check. 1. Remove all the constraints 2. Apply a unit enforced displacement in the x-direction at one selected grid point while constraining the other five components at this selected grid point to zero. This grid point should be close to the center of gravity of the structure, although not a requirement. The x-displacements at all the other grid points should also be equal to unity if the structure is truly unconstrained. If the displacement at a certain grid point is not equal to unity in the x-direction, it is very likely that it overstrained. The likely causes for this can include incorrect modelling of rigid elements, offset beams, non-collinear CELASi. 3. Repeat the same procedure for the other two orthogonal directions. At the conclusion of this check, you should remember to put your original constraints back into your model. 6.3.24.12.2 Automated Rigid Body Method In addition enforced displacement method, you may also request a more robust and more automatic grounding check of the stiffness matrix. This grounding check is also referred to as rigid body check because the stiffness matrix is multiplied by the rigid body transformation matrix. The grounding check identifies unintentional constraints and ill conditioning in the stiffness matrix. Automatic grounding check is requested using the GROUNDCHECK Case Control command. For example, the following command GROUNDCHECK = YES will request a grounding check of the g-set. The following command GROUNDCHECK(SET=ALL) = YES will request a grounding check of all DOF sets. The check may be performed at any or all stages of the stiffness reduction based on the specification of the SET keyword. User Information Message 7570 is issued by GROUNDCHECK for each DOF set requested. The strain energy is computed in each direction of the rigid body motion and by default, if the strain energy exceeds the tolerance, then “FAIL” is printed out for that directory. The tolerance is set by dividing the largest stiffness term by 1.E10. The THRESH keyword specifies the maximum strain energy that passes the grounding check. DATAREC=YES requests data recovery of grounding forces. The RTHRESH=r keyword prints the grounding forces larger than r percent of the largest grounding force if DATAREC is set to YES. 960 Structural Engineering Analysis and Design Second Edition Here is an example for the g-set that indicates the stiffness matrix passes the grounding check in all six rigid body directions. Here is an example for the f-set that indicates the stiffness matrix fails the grounding check in all six rigid body directions. If the DATAREC keyword is specified and the rigid body check fails then data recovery will be performed to compute and print the grounding forces to make it easy to locate the source of the failure. By default, only those grounding forces larger than 10 percent of the largest grounding force will be printed (see RTHRESH keyword). Here is an example of grounding forces created by moving the model in rigid body direction 1 associated with the f-set failure shown above. 6.3.24.12.3 Thermal Equilibrium Method Check against grounding is especially necessary if the structure is subjected to thermal loading. The thermal equilibrium method can actually be used to check against grounding as follows. 1. Remove the actual boundary conditions and apply a set of statically determinate constraints. Typically this procedure is done by constraining all six DOFs at a single grid point. If a single grid point is used, make sure this single grid point contains six degrees of freedom. A single grid point of a model consisting of all solid elements, for example, cannot satisfy this requirement since each grid point of a solid element contains only three degrees of freedom. 2. Change all the thermal coefficients of expansion to a single value. 3. Apply a uniform ∆T to the structure. If the model is “clean,” then the structure should be strain free; in other words, there should be no reaction loads, element forces, or stresses. If this is not the case, then you may want to investigate around the vicinity where the element forces or stresses are nonzero. Incorrect modelling of rigid elements or offsets is a common cause of these types of errors. Once you are satisfied with your model, remember to change the boundary condition, thermal coefficients of expansion, and ∆T back to their original values. 6.3.24.12.4 Load OLOAD and Reaction SPCFORCE Discrepancy using PARAM, PRTRESLT Internal constraints (due to non-colinear CELASi) can also be detected when there is a discrepancy between the OLOAD resultants and SPCFORCE resultants. 961 Structural Engineering Analysis and Design Second Edition 6.3.24.13 Deformed Shape It is very illustrative to inspect the deformed shape DISP (PLOT) in order to ensure that the model correctly simulates the intentions. Deformed Shape ASCII inspection is also recommended and is requested by DISP (PRINT). 6.3.24.14 Massless Mechanisms A massless mechanism mode is defined as a shape that causes very small strain energy when the structure is deflected in this shape. This shape also causes very little kinetic energy when the structure moves in this shape. The ratio of strain energy over kinetic energy is proportional to the eigenvalue of this mode. This result is an indeterminate quantity produced by two terms approaching zero. If applied loads excite this shape small loads can cause very large deflections. If a real mode analysis can be forced to produce a solution in the presence of this condition the mode produced with this shape can have any eigenvalue from positive infinity to negative infinity. These frequencies may change drastically for small changes in the model, or when run on a different computer. Eigensolution failures due to Sturm number inconsistencies are often due to the presence of massless mechanisms. The presence of such modes reduces the reliability and repeatability of eigensolutions and dynamic analysis solutions. A method is now provided to automatically constrain massless mechanisms for eigensolutions, controlled by the user parameter PARAM,MECHFIX,AUTO, which is turned on by default in MSC.Nastran. When this method is used it is unlikely that the eigensolution will fail because of three failed shifts, and the solution produced will be repeatable for small changes in the model, loading condition, or computer type used in the solution. 962 Structural Engineering Analysis and Design Second Edition 6.3.25 Isoparametric Elements and Numerical Integration 22 Most finite elements used in commercial codes are either isoparametric, super-parametric or sub-parametric elements. These elements can map highly distorted curvilinear geometries. An isoparametric element maps the geometry with the same shape functions defining the displacement function. A super-parametric element maps the geometry with a higher order shape function than that which defines the displacement function. Finally, a subparametric element maps the geometry with a lower order shape function than that which defines the displacement function. Super-parametric and isoparametric representation is illustrated for the 3-noded triangle. The superparametric representation is presented as follows. In the super-parametric representation, the triangular coordinates define the element geometry through the first set of relationships. The second set of relationships show the displacement expansion defined by the shape functions, which are in turn expressed in terms of the triangular coordinates. Evidently the element geometry and element displacements are not treated equally. If we proceed to higher order triangles with straight sides, only the displacement expansion is refined whereas the geometry definition remains the same. Elements built according to this prescription are called super-parametric, a term that emphasizes that unequal treatment. The key idea is to use the shape functions to represent both the element geometry and the problem unknowns, which in structural mechanics are displacements. Hence the name isoparametric element (“iso” means equal), often abbreviated to iso-P element. 22 FELIPPA, Carlos A. Introduction to Finite Element Methods. University of Colorado, 2001. 963 Structural Engineering Analysis and Design Second Edition To generalize to include other two-dimensional elements, the term triangular coordinates are replaced by the general term natural coordinates. Natural coordinates (triangular coordinates for triangles, quadrilateral coordinates for quadrilaterals) appear as parameters that define the shape functions. The shape functions then connect the geometry with the displacements. The generalization to an arbitrary two-dimensional element with n nodes is thus presented. Two sets of relations, one for the element geometry and the other for the element displacements, are required. Both sets exhibit the same interpolation in terms of the shape functions. Combining both sets of expressions Thus for the linear (3-noded) triangular element The shape functions are simply the triangular coordinates 964 Structural Engineering Analysis and Design Second Edition Since the resulting expression is the same as that produced by the super-parametric approach, the linear triangle is actually both super-parametric and isoparametric. It is in fact the only triangle that is both super-parametric and isoparametric. The 6-noded triangular element has the following geometric and displacement interpolation where the shape functions are The isoparametric version can thus have curved sides defined by the location of the mid-side nodes. The natural coordinates for a triangular element are the triangular coordinates ζ1, ζ2 and ζ3. The natural coordinates for a quadrilateral element are ξ and η. These are called quadrilateral coordinates. These coordinates vary from -1 on one side to +1 at the other. This particular variation range (instead of, say, 0 to 1) was chosen by the investigators who originally developed isoparametric quadrilaterals to facilitate the use of the standard Gauss integration formulas. The isoparametric 4-noded quadrilateral has the following geometric and displacement interpolation where the shape functions are 965 Structural Engineering Analysis and Design Second Edition The element equilibrium equations can be written for a geometrically linear element to be [ ] {f } = ∫Ω [B A ]T [D A ][B A ]dΩ {d} + {∫Ω [B A ]T {σ}i dΩ}− {∫Ω [B A ]T [D A ]{ε}i dΩ}− {∫Ω [ N]Τ {b} dΩ} Exact integration of the above stiffness matrix and the fixed end forces often cannot be done analytically. Constant strain triangles (CST) have constant [B] and [D] matrices and are a rare exception to the rule since their stiffness and fixed end force matrices can be integrated in closed form. For the quadrilateral, the matrix [B] often depends on the location of the coordinates. This occurs because the shape functions once differentiated are still a function of the natural coordinates. The derivation of the stiffness terms is presented for the isoparametric quadrilateral. Partial derivatives of shape functions with respect to the Cartesian coordinates x and y are required for the strain and stress calculations ultimately to derive the stiffness matrix. Since the shape functions are not directly functions of x and y but of the natural coordinates ξ and η, the determination of Cartesian partial derivatives is not trivial. We require the Jacobian of two-dimensional transformations that connect the differentials of {x, y} to those of {ξ,η} and vice-versa. Hence, the shape function derivatives in terms of the quadrilateral coordinates are or in matrix form These terms feature in the strain matrix [B] which ultimately yields the stiffness matrix [K] for the element. The symbolic inversion of J for arbitrary ξ and η in general leads to extremely complicated expressions unless the element has a particularly simple geometry. This complexity was one of the factors that motivated the use of numerical integration techniques. The use of numerical integration is thus essential for evaluating element integrals of isoparametric elements. The standard practice has been to use Gauss integration (also known as Gauss-Legendre quadrature) because such rules use a minimal number of sample points to achieve a desired level of accuracy. 966 Structural Engineering Analysis and Design Second Edition The Gauss integration rules in one dimension are where p is the number of Gauss integration points (equal of more than one), wi are the integration weights and ξi are the sample point abscissas in the interval –1 to 1. Hence the first four one dimensional Gauss rules are The four rules integrate exactly polynomials in a ξ of orders up to 1, 3, 5 and 7, respectively. In general a onedimensional Gauss rule with p points integrates exactly polynomials of order up to 2p – 1. This is called the degree of the formula. The simplest two-dimensional Gauss rules are called product rules. They are obtained by applying the onedimensional rules to each independent variable in turn. To apply these rules we must first reduce the integrand to the canonical form. 967 Structural Engineering Analysis and Design Second Edition Once this is done we can process numerically each integral in turn. where p1 and p2 are the number of Gauss points in the ξ and η directions, respectively. Usually the same number p = p1 = p2 is chosen if the shape functions are taken to be the same in the ξ and η directions. Hence, if the stiffness matrix is Reducing the integrand into canonical form This matrix function can be numerically integrated over the domain –1 ≤ ξ ≤ +1, –1 ≤ η ≤ +1 by an appropriate Gauss product rule. For square 4-noded quadrilaterals, the integrand h BT EBJ is at most quadratic in ξ and η, and hence 2 x 2 Gauss integration suffice to compute the integral exactly (i.e. the element is fully integrated and not under-integrated). Using a higher order Gauss integration rule, such as 3 x 3 and 4 x 4, reproduces exactly the same stiffness matrix produced by the 2 x 2 integration rule. Using a 1 x 1 rule yields a rank-deficiency matrix. For a non-square quadrilateral, there is little difference in the stiffness matrix beyond the 2 x 2 Gauss integration, with higher Gauss integration orders producing a slightly stiffer response (and hence slightly higher element natural frequencies). 968 Structural Engineering Analysis and Design Second Edition As for the 6-noded triangle, the same stiffness matrix is obtained for integration rule 3, rule -3 or rule 7 as long as the triangular shape is maintained and the mid-side nodes are exactly at the mid-point between corner nodes. A highly distorted triangle on the other hand will return varying stiffness matrices for different Gauss integration rules. A reduced integrated element (Gauss integration of a lower p order) may suffer from matrix singularities as there are insufficient stiffness terms unlike a fully integrated element which will have all its stiffness terms calculated. Under-integrated elements may thus suffer from hourglassing where the deformed shape shows clear zig-zag patterns indicating DOFs which are not stiff. However, often it is usually advantages to use A REDUCED INTEGRATION TECHNIQUE (i.e. the minimum integration requirements that PRESERVES THE RATE OF CONVERGENCE which would result if exact integration were used) as, for very good reasons, A CANCELLATION OF ERRORS due to discretization and due to inexact integration can occur 23. 23 ZIENKIEWICZ, O.C. & TAYLOR, R.L. The Finite Element Method. The Basis. Volume 1. 5th Edition. ButterworthHeinemann, Oxford, 2000. 969 Structural Engineering Analysis and Design Second Edition 6.3.26 Element and Nodal Stress Recovery 24 Stress recovery concepts involve I. stress recovery at the element Gauss points, then II. subsequent stress extrapolation to the element grids, and III. eventually, the (transformation into global coordinates and) averaging of the elemental stresses to yield the grid point stresses 6.3.26.1 Stress Recovery at Gauss Points In the stiffness method, the stresses are obtained from the computed displacements, and are thus derived quantities. The accuracy of derived quantities is generally lower than that of primary quantities (the displacements). For example, if the accuracy level of displacements is 1% that of the stresses may be typically 10% to 20%, and even lower at boundaries. It is therefore of interest to develop techniques that enhance the accuracy of the computed stresses. These procedures receive the generic name stress recovery techniques in the finite element literature. Once the global displacements {U} solved for, and hence the elemental displacements {d} derived, the elemental strain and stress can be obtained from {ε} = [B]{d} {σ} = [D][B]{d} + {σ}i − [D]{ε}i It is of interest to evaluate and report these stresses at the element grid points located on the corners and possibly midpoints of the element. These are called element grid point stresses. It is important to realize that the stresses computed at the same grid point from adjacent elements will not generally be the same, since stresses are not required to be continuous in displacement assumed finite elements. This suggests some form of stress averaging can be used to improve the stress accuracy, and indeed this is part of the stress recovery technique. The results from this averaging procedure are called grid point stresses. Hence to summarize there are the independent element Gauss point stresses, the independent element grid point stresses and the dependent grid point stresses. To obtain the independent element grid point stresses, two approaches are possible, namely (a) Evaluate directly the stress at the element grid locations by substituting the natural coordinates of the grid points as arguments to the shape functions. (b) Evaluate the stress at the Gauss integration points used in the element stiffness integration rule and then extrapolate to the element grid points. Empirical evidence indicates that the second approach generally delivers better stress values for quadrilateral elements whose geometry departs substantially from the rectangular shape. This is backed up by superconvergence (i.e. values sampled at these points show an error which decreases more rapidly than elsewhere) results in finite element approximation theory. Stresses sampled at superconvergent points converge at the same rate as the unknown function or displacement and hence have errors of order O(hp+1). For rectangular elements there is no difference. For isoparametric triangles both techniques deliver similar results (identical if the elements are straight sided with mid-side nodes at midpoints) and so the advantages of the second one are marginal. Hence, on many occasions the displacement or the unknown function is most accurately sampled at the nodes defining the element and the gradients or stresses are best sampled at some interior points. The displacement or unknown function and the stress or the gradients will be exact at the nodes and within the element if the shape function contains the exact theoretical solution to the governing differential equation. When the shape function is of a polynomial of lower order or simply does not contain the exact theoretical solution, the displacement or the unknown function is most accurately sampled at the nodes than anywhere else whilst the stress or the gradients is most accurate at some interior point depending on the order of the element. This can be explained qualitatively as 24 FELIPPA, Carlos A. Introduction to Finite Element Methods. University of Colorado, 2001. 970 Structural Engineering Analysis and Design Second Edition follows. Linear elements such as QUAD4 and TRIA3 have constant first gradient or stress values. If the true stress distribution is linear, the constant FE representation will be exact at the middle of the element. For the quadratic elements of QUAD8 and TRIA6 (with linear FE representation of stress), the 2-point Gauss-Legendre will provide superconvergent sampling of stress. In general, the best accuracy is obtainable for gradients or stresses at the Gauss points corresponding, in order, to the polynomial used in the solution of the unknown function. As far as the optimal points for gradient or stress recovery is concerned, it was observed experimentally by Barlow and proved by Herrmann, that the optimal (not exact because of isoparametric distortion) superconvergent points are the Gauss-Legendre points. This almost always corresponds to the locations of the Gauss-Legendre points for reduced integration (i.e. integration whilst still maintaining the rate of convergence if fully integrated). 6.3.26.2 Extrapolation of Stress From Gauss Points to Element Grids Now that the optimum internal stresses are obtained i.e. at the Gauss points, it is necessary to extrapolate these to the corner and possibly the middle of the element in order to obtain a complete picture. Stress contours are calculated by interpolation involving an extrapolation from the Gauss points to the grids. This means that for element with high stress gradients the interpolated values will be less accurate than for elements with low stress gradients. It is important to check to see what variation of stress exists over the element and if it is large it may be necessary to refine the mesh locally to overcome this problem. Within an isoparametric finite element, stresses are calculated at Gauss points, and are converted from these Gauss point values to grid values. 6.3.26.2.1 Bilinear Extrapolation For QUAD4, had the stresses chosen to be computed at the (non-optimum) 2 x 2 Gauss integration points, each stress component is “carried” to the corner nodes and the center of the element through a bilinear extrapolation based on the computed values at the Gauss points. The optimum superconvergent Gauss point for a QUAD4 is at the center. Here we are only demonstrating the principle of bilinear extrapolation. To understand the extrapolation procedure more clearly it is convenient to consider the region bounded by the Gauss points as an “internal element” or “Gauss element”. The Gauss element, is also a four-node quadrilateral. Its quadrilateral (natural) coordinates are denoted by ξ’ and η’. These are linked to ξ and η by the simple relations Any scalar quantity w whose values wi’ at the Gauss element corners are known can be interpolated through the usual bilinear shape functions now expressed in terms of ξ’ and η’. 971 Structural Engineering Analysis and Design Second Edition To extrapolate w to corner 1, say, we replace its ξ’ and η’ coordinates, namely ξ’ = η’ = -31/2, into the above formula. Doing that for the four corners we obtain Note that the sum of the coefficients in each row is one, as it should be. Also, note that each stress component is extrapolated independently. 6.3.26.2.2 Superconvergent Patch Recovery (SPR) method (ZIENKIEWICZ, 2000) This is a highly efficient method of stress extrapolation. 6.3.26.2.3 Recovery by Equilibration of Patches (REP) method (ZIENKIEWICZ, 2000) This is a highly efficient method of stress extrapolation. 6.3.26.3 (Transformation into Global Coordinates and) Averaging of the Elemental Grid Stresses to Yield the Grid Point Stresses The stress is calculated on an element by element basis (unlike the displacement) so it is possible, and in fact very likely, that the stresses at a grid in one element will not match up with the stress at the same grid in an adjacent element (irrespective of whether the elemental stress is calculated directly at the grids or by extrapolation from the Gauss points). In some cases, where there is a discontinuity in the material properties or the thickness of the elements, it is correct that there is a local stress discontinuity, however in other cases this stress difference will be a measure of the error in the solution. When contour plots of the stresses are required, or when a stress value is required for design purposes it is better to have a single value. The values from all the adjacent independent elements grid point stresses at a grid can be averaged to give a single value at the grid, i.e. the dependent grid point stresses. This averaging can be weighted based on the element type, geometry etc. if required. Typically the determinant of the Jacobian divided by the total element volume is used as the basis of the weighting function since this will emphasize those elements that have a large amount of material related to the node at the expense of those elements that are rather elongated. However it should be remembered that the stresses, which look smooth and continuous on the plots, are in fact calculated as a series of discontinuous stress patches. As the mesh is refined, the element stress values will tend to converge. Hence, the averaged grid point stress can be used as an error estimator. The averaging of the element grid stresses is best performed in the post-processor. Averaging SHOULD NOT be performed between dissimilar element types, between shells of differing thickness, beams of differing cross sections nor between elements of different material properties. 972 Structural Engineering Analysis and Design Second Edition 6.3.26.4 Element Stress Recovery Procedures in MSC.NASTRAN 6.3.26.4.1 CQUAD4 Elements CENTRE method requests element stress recovery at center only. This is the default for QUAD4 elements and is the optimum sampling point. This is requested with ELSTRESS (CENTER). BILINEAR stress recovery procedure requests stress recovery at center and at element grids. This is requested with ELSTRESS (CORNER). This method uses the results at the gauss points to create a linear function that is then used to extrapolate the results out to the grid points. In the case of a linear varying moment in a cantilevered engineering beam model, since the QUAD4 element is an almost constant strain curvature element, the gauss results are constant curvature in each element, thus the linear function is almost constant curvature for each element, thus the CORNER strain curvatures are almost constant in an element, hence the reason for the CENTER method being the default for QUAD4. In a cantilevered beam problem, corner stress output using the bilinear method will cause a step function from the cantilever point to the load application point, which is obviously a coarse approximation of the correct linear stress distribution of the engineering model. To conclude, the bilinear corner stress option uses the grid displacements to interpolate strains to gauss points using the element shape functions. Stresses are then calculated at these gauss points. Finally, these stresses are extrapolated to grids using a bilinear stress function. CUBIC stress recovery requests stress recovery at the grids directly without calculating at the Gauss points; In MSC.NASTRAN the CUBIC method works from the grid displacements. It uses the grid displacements and rotations to curve-fit a cubic equation to develop the element strain/curvature distribution. In the case of a linear varying moment in the cantilevered beam engineering model, since the grid point rotations vary across the element, the curve fit gives the correct engineering result of a linearly varying strain curvature across the QUAD4 element, which translates to a linear varying stress. This method is much like the cubic beam stress recovery. SGAGE stress recovery requests stress recovery at the grids directly without calculating at the Gauss points; In MSC.NASTRAN, the SGAGE method is similar to the CUBIC method in that grid displacements are used, but inplane strains and curvatures are calculated independently. First strains are calculated in the u and v and diagonal uv directions at each grid point. The state of in-plane strain at the grid point is calculated using rosette strain gauge equations. Grid strain curvatures are done similarly. The resulting grid point strain and curvature states can then be changed to forces and stresses at the grid points. The BILINEAR option is the default because it is the most stable in all cases, but as is shown in the linearly varying moment case, it can be much less accurate than the CUBIC method. The CUBIC method is very accurate if the mesh if fine enough to give accurate displacements. However, coarse meshes can cause the cubic curve-fit to be more inaccurate than the BILINEAR method. The SGAGE method is similar to the CUBIC method but not as accurate and is quite obsolete. Stiffness matrix integration and stress calculation need not necessarily use the same Gauss Quadrature Rule, i.e. the stresses may be calculated at the more accurate (superconvergent) lower order Gauss Rule and the stiffness fully integrated. Because we know that the (fully integrated) stress variation of the finite element is not good enough to capture variation in reality, we use reduced integration stress recovery techniques, as recovery is best at the lower order Gauss points. This is what happens with the BILINEAR, SPR and REP recovery methods; not with CUBIC or SGAGE methods which do not extrapolate stresses from the Gauss points, instead calculates stresses from the displacements and rotations at the nodes. Hence, we can say that BILINEAR, SPR or REP are better when the fully integrated stress variation is not good enough, but CUBIC or SGAGE is better when the fully integrated stress variation is good enough to model reality. In any case, the results should converge with refinement of the mesh. Reiterating, BILINEAR is the superconvergent reduced integrated (although can be fully integrated as well if the finite element variation is deemed accurate enough to model reality) stress recovery (i.e. stress recovery at Gauss points based on, the not so high order polynomial, shape functions defined by the displacement unknowns; then 973 Structural Engineering Analysis and Design Second Edition extrapolation from Gauss points), and CUBIC is the (fully integrated) stress recovery (i.e. stress recovery not at Gauss points but throughout the element based on shape functions defined by the unknowns). Hence, we can say that the reduced integrated BILINEAR is better when the fully integrated stress variation is not good enough, but CUBIC is better when the fully integrated stress variation is good enough to model reality. In any case, the results should converge with refinement of the mesh. The ELSTRESS (CENTER) outputs the σx, σy and τxy stresses in the element coordinate system (MCID field of CQUAD4) at the center of the element on the top and bottom surfaces. The ELFORCE (CENTER) outputs the membrane forces per unit length Fx, Fy, and Fxy, bending moments per unit length Mx, My and Mxy and transverse shear forces per unit length Qx and Qy, all in the element coordinate system at the center of the element. The ELSTRESS (CORNER) outputs the σx, σy and τxy stresses in the element coordinate system at the center and 4 corners of the element on the top and bottom surfaces. 974 Structural Engineering Analysis and Design Second Edition The ELFORCE (CORNER) outputs the membrane forces per unit length Fx, Fy, and Fxy, bending moments per unit length Mx, My and Mxy and transverse shear forces per unit length Qx and Qy, all in the element coordinate system at the center and 4 corners of the element. Note that the options CENTER or CORNER are not applicable to elements other than QUAD4. 6.3.26.4.2 CQUAD8 The ELSTRESS outputs the σx, σy and τxy stresses in the element coordinate system at the center and 4 corners of the element on the top and bottom surfaces. The ELFORCE outputs the membrane forces per unit length Fx, Fy, and Fxy, bending moments per unit length Mx, My and Mxy and transverse shear forces per unit length Qx and Qy, all in the element coordinate system at the center and 4 corners of the element. 975 Structural Engineering Analysis and Design Second Edition 6.3.26.4.3 CTRIA3 The ELSTRESS outputs the σx, σy and τxy stresses in the element coordinate system at the center of the element on the top and bottom surfaces. The ELFORCE outputs the membrane forces per unit length Fx, Fy, and Fxy, bending moments per unit length Mx, My and Mxy and transverse shear forces per unit length Qx and Qy, all in the element coordinate system at the center of the element. 6.3.26.4.4 CTRIA6 The ELSTRESS outputs the σx, σy and τxy stresses in the element coordinate system at the center and 3 corners of the element on the top and bottom surfaces. The ELFORCE outputs the membrane forces per unit length Fx, Fy, and Fxy, bending moments per unit length Mx, My and Mxy and transverse shear forces per unit length Qx and Qy, all in the element coordinate system at the center and 3 corners of the element. 6.3.26.4.5 CHEXA4, CHEXA20, CPENTA6, CPENTA15, CTETRA4, CTETRA10 The ELSTRESS outputs the σx, σy ,σz, τxy ,τzx and τyz stresses in the element, basic (default) or material (depending on CORDM field of the PSOLID entry) coordinate system at the center and either the corners (default) or the Gauss points (depending on PSOLID entry) of the element. 976 Structural Engineering Analysis and Design Second Edition 6.3.26.5 Grid Point Stresses in MSC.NASTRAN Although it is usual to perform the grip point stress calculation in the post-processor, it is instructive to know that MSC.NASTRAN also has the feature of calculating grid point stresses. Moreover, the methods used within the post-processor are usually similar. The grid point stress option calculates the stresses at the grid points from the adjoining plate and solid elements in the global or a user defined coordinate system. Each stress component (e.g. σx) is treated independently of other stress components in the calculation of average grid point stress components. The stress invariants at grid points (i.e., principal stresses, the Hencky-von Mises stress, and the mean pressure) are evaluated from the average values of the stress components at the grid points. Most element have vertex element stress (i.e. element grid point stress) values. These include CQUADR, CQUAD4 (with corner option), CQUAD8, CTRIAR, and CTRIA6 shell elements as well as the CHEXA, CPENTA, and CTETRA solid elements. But not CQUAD4 (without corner option) and CTRIA3. Two methods are used to calculate grid point stress components for plate and shell elements namely, topological and geometric, with topological as the default method. Topological Geometric Averages stresses at grids with element vertex stresses, ignores CQUAD4 (without corner option) and CTRIA3. Grids with only CQUAD4 (without corner option) and/or CTRIA3, average of center stress used. Hence no element size consideration. Averages stresses at grids with element vertex stresses, ignores CQUAD4 (without corner option) and CTRIA3. Grids with only CQUAD4 (without corner option) and/or CTRIA3, average stress obtained from least square approximation. Hence size of element considered. Recognizes stresses at interior, corner, or edge grid points to be continuous between directly connected elements. Recognizes stresses at exception grid points to be discontinuous (large slope between adjacent elements cause stress discontinuities) between connected elements and, a different grid point stress may be output for each of the connected elements. Recognizes stresses at interior, corner, or edge grid points to be continuous between directly connected elements. Does not recognize exception grid points. User defined separate surface sets adjacent to exception grids required. If the results are substantially different when using the two different methods, it may be an indication that the FE model is not fine enough. In general, if the FE model is fine enough to capture the stress gradients, the two methods should yield similar results. The NASTRAN request interface is as follows. $ CASE CONTROL ELSTRESS (PLOT) = ALL $ Required $ SET 10 = < SURFACE IDs > say < 100, 200 > GPSTRESS = 10 $ Printed Output of Grid Point Stresses STRFIELD = 10 $ Graphical Output of Grid Point Stresses $ OUTPUT(POST) SET 1 = < Element IDs > For shells, Z-normals (defining top and bottom SET 2 = < Element IDs > surfaces) are required. Specify VOLUME for solids. SURFACE 100 SET 1 NORMAL Z SURFACE 200 SET 2 NORMAL Z The element positive normal is in the direction of the z-axis of the basic coordinate system. By default, the grid point stresses are transformed to the basic coordinate system. The grid point stresses are called out by the GPSTRESS command, which points to set 10, which, in turn, points to surfaces 100 and 200. 977 Structural Engineering Analysis and Design Second Edition The GPSTRESS output is presented as follows. 978 Structural Engineering Analysis and Design Second Edition 6.3.27 Full Integration Quadrature, Reduced Integration Quadrature and Optimal Gauss Sampling Points It is usually advantages to use A REDUCED INTEGRATION TECHNIQUE (i.e. the minimum integration requirements that PRESERVES THE RATE OF CONVERGENCE which would result if exact integration were used) as, for very good reasons, A CANCELLATION OF ERRORS due to discretization and due to inexact integration can occur 25. As far as the optimal points for gradient or stress recovery is concerned, it was observed experimentally by Barlow and proved by Herrmann, that the optimal (not exact because of isoparametric distortion) superconvergent points are the Gauss-Legendre points. This almost always corresponds to the locations of the Gauss-Legendre points for reduced integration (i.e. integration whilst still maintaining the rate of convergence if fully integrated). Element Displacement Variation Fully Integrated Stress Variation y = constant + x + x2 + x3 Complete 3rd order My, Mz linear in x; Vy, Vz constant in x; Ax constant in x; Tx constant in x; In-plane C0 Linear TRIA3 (CST) u = constant + x + y v = constant + x + y Complete 1st order σx, σy and τxy constant is x and y In-plane C0 Parabolic TRIA6 (LST) u = constant + x + y + x2 + xy + y2 v = constant + x + y + x2 + xy + y2 Complete 2nd order σx, σy and τxy linear is x and y In-plane C0 Linear QUAD4 u = constant + x + y + xy v = constant + x + y + xy Complete 1st order; Incomplete 2nd order σx constant in x, linear in y; σy constant in y, linear in x; τxy linear is x and y Two-noded C1 Cubic Beam In-plane C0 Parabolic QUAD8 (Serendipity) Out-of-plane C1 Kirchhoff QUAD4 Out-of-plane C0 Mindlin QUAD4 Out-of-plane C0 Mindlin QUAD8 Linear TETRA4 u = constant + x + y + xy + x2 + xy + y2 + x3y v = constant + x + y + xy + x2 + xy + y2 + xy3 Complete 2nd order; Incomplete 3rd order w = constant + x + y + x2 + xy + y2 + x3 + y3 + x2y + xy2 + x3y + xy3 Complete 3rd order σx linear in x, parabolic in y; σy linear in y, parabolic in x; τxy parabolic in x, y Fully Integrated Gauss Quadrature 2 Reduced Integrated Stress Variation 2 My, Mz linear in x; Vy, Vz constant in x; Ax constant in x; Tx constant in x; Both 1 x 1 Rule 3 or –3 Optimal Sampling Reduced Integration 2x2 Both 1 x 1 3x3 Both 2 x 2 2 x 2 bending 2 x 2 shear 1 x 1 or 2 x 2 bending 1 x 1 shear σx, σy and τxy constant in x and y σx, σy and τxy linear in x and y σx, σy and τxy constant in x and y σx, σy and τxy linear in x and y σx linear in x σy linear in y 3 x 3 bending 3 x 3 shear u = constant + x + y + z v = constant + x + y + z w = constant + x + y + z Complete 1st order Optimum Superconvergent Sampling Points (Reduced Integration Gauss Quadrature) 2 x 2 or 3 x 3 bending 2 x 2 shear 1x1x1 σx, σy constant σx, σy linear σx, σy, σz, τxy, τyz, τzx constant 25 ZIENKIEWICZ, O.C. & TAYLOR, R.L. The Finite Element Method. The Basis. Volume 1. 5th Edition. ButterworthHeinemann, Oxford, 2000. 979 Structural Engineering Analysis and Design Second Edition Parabolic TETRA10 Linear HEXA8 Parabolic HEXA20 u = constant + x + y + z + xy + yz + zx + xyz v = likewise w = likewise Complete 1st order; Incomplete 2nd order u = constant + x + y + z + x2 + y2 + 2 z2 + xy + yz + zx + x2y + xy2 + y z 2 2 2 2 + yz + z x + zx + xyz + x yz + 2 2 xy z + xyz v = likewise w = likewise Complete 2nd order; Incomplete 3rd order 980 2x2x2 1x1x1 3x3x3 2x2x2 Structural Engineering Analysis and Design Second Edition 6.3.28 Stress Interpretation Stress recovery concepts, namely I. stress recovery at the element Gauss points, then II. subsequent stress extrapolation to the element grids, and III. eventually, the (transformation into global coordinates and) averaging of the elemental stresses to yield the grid point stresses have been covered. Here we shall focus on the engineering interpretation of these stresses. A solid element outputs (the appropriate variations of) 3 normal stresses and 3 shear stresses σxx , σyy , σzz , τxy , τyz , τzx in its element coordinate system. A shell element outputs (the appropriate variations of) 2 normal stresses and 1 shear stress σxx , σyy , τxy in its element coordinate system. A beam element outputs (the appropriate variations of) 2 bending moments Myy and Mzz, 2 shear forces Fy and Fz, 1 torsional moment Mxx and 1 axial force Fx. Stresses from solids and shells can be cumulated into forces if the design criteria are specified (as is usual for composite material such as reinforced concrete) in terms of moments, shear and axial forces. Conversely, forces from beam elements can be used to derive stresses based on simple bending theory. Element stress recovery is (unless otherwise specified) done in the element coordinate system. To define a beam, the two end nodes define the x-direction of the element from node 1 to node 2. The third node defines either its yor z-axis. To define shells, the direction of the node number definitions defines the element x- and y-axes. The zaxis is then automatically defined using the Right Hand Rule usually. Likewise, for solids, the numbering of the nodes will define the x-, y- and z-axes. A preprocessor should be used to plot the element coordinate systems for all the elements (ensuring that it is consistent with the element coordinate definition of the particular code). For beams, the elements X-, Y- and Z- axes must be orientated in the same manner. Stress recovery is performed in the beam local element system. No transformation into a global system is performed, hence the requirement for the elements to be orientation consistently for the bending moment and shear force diagrams about and in the two directions to look consistent between elements. For shells, the element Z-normals must be consistent. This is because the top and bottom surface stresses need to be viewed consistently. Stress recovery is performed in the element coordinate system by default (but defined by MCID entry on element connection card; 0 for basic projected, > 0 for user projected, < blank > for element coordinate system, > 0.0 and < 360.0 for angled from side n1-n2 of element). The element results are then usually transformed into the global coordinate system. Of course, unless the results are transformed into the global coordinate system, the definition of the X- and Y- element coordinate system between elements of the same type must also be consistent. Alternatively, a random element X- and Y- orientation (but consistent Z-normals of course) can be used between elements of the same type if after stress recovery, the output is transformed (by the post-processor) into the global coordinate system. For solid elements, the stress recovery is performed in the basic coordinate system by default (but defined on CORDM field of PSOLID; 0 for basic, > 0 for user-defined, -1 for element coordinate system). Hence, if the stress recovery is presented in the basic coordinate system, a random X-, Y-, Z- element orientation can be used. To conclude, the element X-, Y- and Z- orientation for beams must be consistent as stress recovery is presented in the element coordinate system, the Z-normal for shells must be consistent but the element Xand Y- orientation can be random as long as the stress recovery is presented in the global coordinate system, and for solids a random X-, Y- and Z- element orientation is fine as long as the stress recovery is presented in the global coordinate system. Note that although the element stress tensors σxx , σyy , σzz , τxy , τyz , τzx must be viewed in a consistent coordinate system, derived quantities are independent of the element orientation. These invariant quantities included maximum and minimum principal stresses, maximum shear stress and the von Mises stress. 981 Structural Engineering Analysis and Design Second Edition 6.3.28.1 State of Stress i.e. Global Coordinate Stress Tensors σxx , σyy , σzz , τxy , τyz , τzx Normal stresses are normal to the plane and shear stresses act on the plane. The first subscript in the stress notation denotes the direction of the normal to the plane on which the stress acts and the second subscript indicates the direction of the stress itself. In shells and solids, stresses in the element coordinate system are usually quite meaningless. The state of stress (three normal and three shear stresses in general) at a point with reference to the global Cartesian system is also quite insignificant in its original form. However, the various derived stress quantities, which can be obtained, are very illustrative. These are presented as follows. (i) The load path of flow of stresses through the structure can be ascertained very intuitively from the principal normal stresses σ1 , σ2 and σ3. When an element is orientated such that all its shear stress components are zero, the normal stresses on its 3 planes are called the principal stresses σ1, σ2 and σ3 from most positive to most negative. When one of the principal stresses are zero, the stress state is biaxial (or plane stress). When two of the principal stresses are zero, the stress state is then uniaxial. Let us assume tensile as positive. σ2 and σ3 that is close to zero indicates a state of uniaxial tensile stress if σ1 positive. σ2 and σ1 that is close to zero indicates a state of uniaxial compressive stress if σ3 negative. Note that the principal stress orientation is a function of loading, not geometry alone. Hence, a plot of principal stresses is dependent upon a particular load case. The direction of flow of stresses (if tensile) is a good indication of the optimum direction of reinforcement to be provided in reinforced concrete. Flows of Stresses i.e. Principal Stresses on a Structural Connection Casting (ii) The state of overall stress, i.e. compressive or tensile can be ascertained from the average stress. (iii) The susceptibility of the structure to a specified failure mode can be assessed. 982 Structural Engineering Analysis and Design Second Edition 6.3.28.2 Failure Criteria The applicable failure criterion for a particular material depends on whether the material is ductile or brittle. Ductile materials yield and then undergo significant plastic deformation before ultimate fracture. Brittle materials do not yield and undergo plastic deformation, but fractures when the ultimate strength is attained. Carbon steel and aluminium are generally ductile materials whilst concrete, masonry, quenched tempered alloy steel, hardened tool steel and gray cast iron are brittle materials. Of course, certain composite materials such as reinforced concrete and reinforced masonry can be deemed to be ductile materials. However, some materials become more brittle as the strain-rate increases and temperature decreases. Some metals such as copper and aluminium have a crystalline structure that enables them to resist fast fracture under all loading conditions and at all temperatures. This is not the case with ferrous alloys, particularly structural steel which is brittle below the transition temperature. Ductile materials usually have approximately the same ultimate tensile and compressive strengths. Brittle materials on the other hand are usually stronger in compression than in tension. For instance, the ultimate compressive strength of gray cast iron can be 3 to 4 times its ultimate tensile strength. There are exceptions, for instance the brittle hardened tool steel which has similar ultimate strengths in both tension and compression. If the percentage elongation in a tensile test is less than 5% at ultimate strength or if there is no published yield strength, then assume brittle behaviour. It will be shown that ductile materials tend to yield along 45° shear slip planes at the same pure normal stress, whether in tension or compression, i.e. if a ductile specimen were to be loaded in tension to fracture, the fractures will all be at an angle of approximately 45° from the loading axis. On the other hand, a tensile specimen of brittle material does tend to fail in tension (i.e. fracture on a plane orthogonal to the maximum principal tensile stress) and in shear at approximately 45° angles when loaded to fracture in compression. 983 Structural Engineering Analysis and Design Second Edition 6.3.28.2.1 Ductile Yielding (Plastic Flow) Failure Criteria A yielding failure occurs when the material yields such that it compromises the performance of the structure in its load carrying capacity. Localized yielding around stress concentrations may be acceptable as a ductile material is capable of redistributing the stresses sufficiently for yielding to stop at a distance from the concentration whilst not compromising the integrity of the structure. The ductile failure theories are as follows. σ2 σy Maximum Shear Stress (Tresca) Failure Criterion Von Mises Failure Criterion σ1 σy −σy −σy Tresca is the safest criterion, but the best match to experimental data is the von Mises criterion. Any of these failure criteria can be employed on a set of loadcases and enveloped. Principal Normal Stress Failure Criterion Principal Normal Stresses σ1 , σ2 and σ3 Failure Criterion The principal normal stresses are the maximum, minimum and intermediate normal stresses that occur when the element is rotated onto its principal plane. The shear stresses are zero on these principal planes. Visualize the 3dimensional Mohr Circle of stresses (3 circles). The principal stresses in two dimensions are presented, as is that in three dimensions as a solution of a 3rd order equation. σ 3 + I1σ 2 + I 2 σ − I 3 = 0 σ1, 2 = σ x + τ xy 2  σx − σy ±  2  2   + τ xy 2  where I1 = σ x + σ y + σ z I 2 = σ x σ y + σ y σ z + σ z σ x − τ xy − τ yz − τ zx 2 2 2 I 3 = σ x σ y σ z + 2τ xy τ yz τ zx − σ x τ yz − σ y τ zx − σ z τ xy 2 2 2 The maximum normal stress failure criterion states that failure occurs whenever σ1 or σ3 equals the failure strength of the material in tension or compression, respectively. For ductile materials, failure by yielding occurs when the yield strength is attained whilst failure by fracture occurs when the ultimate strength is reached. Ductile materials have approximately the same ultimate tensile and compressive strengths. This theory however does not account for the entire complex triaxial stress state and hence assumes that yielding (flowing) occurs either along the direction of the maximum principal stress or the minimum principal stress. A plot of the maximum principal stress (tension) and the minimum principal stress (compression) can be generated for all load cases and enveloped. Maximum and Minimum Principal Stresses on a Structural Connection Casting 984 Structural Engineering Analysis and Design Second Edition Von Mises-Hencky (Distortion Energy) Stress σvon mises Failure Criterion The von Mises (or effective stress) stress is a measure of the distortional stresses. It gives a good indication of how close a material is to yielding or experiencing plastic flow. It is based upon strain energy hypothesis and represents the entire complex triaxial stress state. This yield criterion is suitable for pressure independent material models i.e. materials that will not flow (fail) under the conditions of hydrostatic stress. With this material model the yield surface is independent of pressure (average stress). This is typical of materials such as steel. The material yields when the von Mises stress reaches the one-dimensional yield strength, σvm = σy or, alternatively in terms of principal stresses The von Mises model provides the best match to experimental data of failure limits. A plot of the von Mises state of stress can be generated for all load cases and enveloped. Von Mises on a Structural Casting, σvm < σy = 350MPa OK Maximum Shear Stress (Tresca) Failure Criterion The Tresca yield criterion is based on the maximum shear stress and is especially useful for predicting the yielding of annealed ductile materials. The Tresca criterion specifies that if any stress component exceeds the specified yield strength, the material will flow (undergo plastic deformation). It is more conservative than the principal normal stress and the von Mises stress failure criteria. The Tresca criterion states that failure by yielding occurs on a shear slip plane i.e. at 45° to the principal planes when the maximum shear stress equals ½ the yield strength. τ13 = (σ1 − σ3)/2 = σy/2 The theory is suggested by the fact that yielding is related to shear slip (at the plane of maximum shear stress which is 45° to the planes of the maximum and minimum principal stresses) at the atomic level of the material. A plot of the maximum shear stress τ13 of stress can be generated for all load cases and enveloped. Tresca Failure Criterion: Max Shear Stress, τ13 = (σ1 − σ3)/2 < σy/2 = 175MPa OK 985 Structural Engineering Analysis and Design Second Edition 6.3.28.2.2 Brittle Fracture (Frictional) Failure Criteria Brittle fracture occurs when the material cracks such that it becomes detrimental to the structural performance in its load carrying capacity. Fracture occurs when cracks appear without significant permanent (plastic) deformation. Principal Normal Stresses σ1 , σ2 and σ3 Failure Criterion The maximum normal stress failure criterion states that failure occurs whenever σ1 or σ3 equals the failure strength of the material in tension or compression, respectively. For brittle materials, failure by fracture occurs when the ultimate strength (not yield strength as in ductile materials) is attained. Brittle materials are usually stronger in compression than tension. Fracture is deemed to occur either in the plane normal to the maximum tensile stress for a tensile failure or in a plane oblique to the maximum compressive stress as what appears to be a shear fracture (but not as a rule on the plane of maximum shear stress) for a failure in compression. Mohr-Coulomb Failure Criterion Brittle materials such as concrete, soil, gray cast iron and hardened tool steel are held together by frictional forces and they fail by sliding. The effect of the stress normal to the failure plane is important and should be included in the failure criterion. Fracture occurs when the maximum and minimum principal stresses satisfies the following equation. (σ1 / σut) − (σ3 / σuc) > 1.0 where σut and σuc the represent the ultimate tensile and compressive strengths. τ φ σuc σ3 σ1 σ σut This theory is best used in brittle materials that are much stronger in compression. The Mohr-Coulomb equivalent stress is analogous to the Tresca failure criterion but incorporates the effect of the normal stress, unlike Tresca, which is pressure independent. Fracture is deemed to occur either in the plane normal to the maximum tensile stress for a tensile failure or in a plane oblique to the maximum compressive stress as what appears to be a shear fracture (but not as a rule on the plane of maximum shear stress) for a failure in compression. A special case occurs in certain brittle materials such as hardened tool steel where the ultimate strengths are the same both in tension and compression. In this case the criteria becomes (σ1 / σut) − (σ3 / σuc) < 1.0 (σ1 / σu) − (σ3 / σu) < 1.0 σ1 − σ3 < σu which is exactly similar (in expression only) to the ductile (maximum shear stress) Tresca τ13 = (σ1 − σ3)/2 = σy/2 criteria. Of course the mode of failure remains different in the brittle material (plane normal to the maximum tensile stress for a tensile failure or in a plane 45° oblique to the maximum compressive stress) compared to ductile materials (45° to principal planes for failure in either tension or compression). But the fact remains that the maximum shear stress can be plotted on a post-processor to determine if the special equal (in tension and compression) strength brittle material meets the Mohr-Coulomb criterion or not. 986 Structural Engineering Analysis and Design Second Edition BS 5950-Part1:2000 (cl. 2.4.4) Criterion Brittle fracture is used to describe fast unstable fractures, in contrast to stable fractures such as fatigue or slow unstable fractures such as plastic yielding. Some metals such as copper and aluminium have a crystalline structure that enables them to resist fast fracture under all loading conditions and at all temperatures. This is not the case with ferrous alloys, particularly structural steel. The Liberty ships and the King Street bridge in Melbourne, the Sea Gem drilling rig for North Sea gas and the Alexander Kielland oil rig are a few examples of the casualties of brittle fracture. An important feature of steel is the transistion temperature between ductile and brittle fracture. To determine the risk of brittle fracture, the following are considered: I. minimum operating temperature II. thickness of material to be used III. steel grade IV. stress level V. detail; parent plate, weld metal or heat affected zone HAZ, holes VI. strain-rate In addition, the welding electrodes or other welding consumables should have a specified Charpy impact value equivalent to, or better than, that specified for the parent metal. BS 5950-Part 1:2000 (cl. 2.4.4) gives maximum permissible thicknesses of steel at given operating temperatures based on Charpy toughness energy absorption impact tests. The steel quality selected for each component should be such that the thickness t of each element where t1 is the limiting thickness at the appropriate minimum service temperature Tmin for a given steel grade and quality where Tmin is the minimum service temperature, Ynom is the nominal yield strength for thickness < 16mm for the steel grade used and T27J is the test temperature at which 27J Charpy value was obtained as according to Table 7. Table 4 and Table 5 presents the calculated the t1 values. 987 Structural Engineering Analysis and Design Second Edition K is a factor that depends on the type of detail, the general stress level, the stress concentration effects and the strain conditions. Values are given in Table 3. In addition, the maximum thickness of the component should not exceed the maximum thickness t2 at which the full Charpy impact value applies to the selected steel quality for that product type and steel grade, according to the relevant product standard, see Table 6. 988 Structural Engineering Analysis and Design Second Edition 6.3.28.2.3 Large Deflections due to Insufficient Stiffness The structure may be deemed to fail if certain sections deform considerably (static or dynamic response may be too high) under the applied excitation such that it fails to meet the required deflection tolerance criteria. 6.3.28.2.4 Buckling Buckling is the sudden loss of stability or stiffness under the applied loads. The stress levels may not even be sufficiently high for failure by yielding to occur, in which case a linear elastic buckling analysis will predict this failure. See Section 3.2. 6.3.28.2.5 Fatigue Components subject to repetitive cycles of loading may fail after a certain number of cycles. A pseudo-static or dynamic fatigue analysis is required to predict this failure. See Section 5.5. 6.3.28.2.6 Creep or Viscoelasticity Structures under load gradually deform over time. This may be accounted for by modifying the stiffness modulus with an apparent creep modulus. Creep or viscoelasticity is a time dependent, plastic deformation under sustained load. The amount of creep experienced is a function of time, temperature and applied load. Creep is more significant for plastics even under room temperature. Creep is not significant for most metals until operating temperatures reach 35 to 70 percent of respective melting points. 989 Structural Engineering Analysis and Design Second Edition 6.3.28.3 Deriving Forces (Moments, Shear, Torsion & Axial Force) from Stresses in Shells Moments, shear, torsion and axial forces are usually the design criteria for composite material such as reinforced concrete. Hence, to facilitate the design of these structural elements, often the computed stresses are summed to obtain the equivalent averaged forces. The stresses and hence forces obtained from a shell is summarized as follows. Zero for shells The output stresses are the in-plane normal stresses σxx and σyy, varying linear through the thickness the in-plane shear stresses τxy, varying linearly through the thickness the out-of-plane shear stresses τxz and τyz, constant through the thickness although from equilibrium considerations, they should vary parabolically From these, the in-plane force tensors Nx, Ny and Nxy, the bending tensors Mx, My and Mxy and the throughthickness shear force vectors Qx and Qy. These simplify to Note that these are forces and moments based on the stresses and hence act over the same width that the stresses act. For design purposes, often a per meter width design moment and force are required. Hence, the values of moments and forces of all elements over the physical width of a meter should be averaged for the design values. On a further note on design, the complications of designing for the torsional moment (derived from the in-plane bending shear stresses) Mxy is avoided by increasing the design moments Mxx and Myy as follows. 990 Structural Engineering Analysis and Design Second Edition 6.3.29 The Element Strain Energy Density The element strain energy is basically the elastic energy stored in the structural element. As an example, if you hold onto one end of the spring and push slowly on the other end starting from rest, the load deflection curve looks as follows for small deflections. The strain energy U = 0.5Fδ = 0.5kδ2. The strain energy distribution within a structure denotes the elements that are working the hardest, i.e. the higher the strain energy, the harder the element is working. Hence, for a given loadcase it provides information on the elements that should be stiffened to increase the overall stiffness (and hence to minimize the deflections) to that loadcase. The required request in MSC.NASTRAN is $ CASE CONTROL SECTION ESE() = ALL/ To illustrate this concept, consider the following springs in series. The goal is to reduce the tip deflection at grid point 2. Without performing any calculation, it is quite obvious that stiffening K2 is more efficient than stiffening K1. The next step is to calculate the strain energy and see if it also guides you in the same direction. The deflections and element strain energy are Since U2 is an order of magnitude greater than U1, clearly it is better to stiffen K2 than K1 to reduce the deflections at the tip. The element strain energy distribution for a car model is shown below (courtesy of Lapcad Eng). The strain energy density is an effective design tool for linear static analysis (SOL 101), buckling analysis (SOL 105 and SOL 106) and for dynamic linear modal analysis (SOL 103). 991 Structural Engineering Analysis and Design Second Edition The ESE request outputs the following. 992 Structural Engineering Analysis and Design Second Edition 6.3.30 Error Estimation 6.3.30.1 GL, ML Analysis Error Estimation: h- or p- Refinement Finite elements attempt model a continuum with discrete parameters, i.e. a finite number of DOFs. As long as the following conditions are met (i) the analysis is linear (ii) the finite elements are based on the variational approach (or the Galerkin approach) (iii) the geometry and material properties are represented accurately (iv) continuity requirements of the shape functions are satisfied (v) the integration of the discrete system of equations is accurate (vi) all essential boundary conditions are associated with zero values the work done by the total nodal loads due to nodal displacements as predicted by the discrete system will always be less or equal to the exact value {{f+P)T{u}}discrete ≤ {{f+P)T{u}}discrete Hence, the discrete structural analysis based on a finite number of DOFs will always present a stiffer response than the exact solution provided the above conditions are met. Hence, a finer mesh will generally be associated with a more flexible response and hence a closer to exact approximation. The stiffer response occurs due to the fact the that the chosen shape functions cannot represent all the possible modes of deformation of the structure. A useful method of approximate error estimation is described as follows. The approximate order of error has been established, but not the percentage of error itself relative to the exact solution. We shall illustrate the principle for the in-plane displacement and strain or stress of a triangular (or rectangular for that matter) finite element. {{f+P)T{u}} Exact Solution Element Size h h/2 An estimate of the exact solution can be obtained by performing two linear analyses with either h- or p-refinement. Employing h-refinement, we can establish the estimate of the exact displacement and stress (or strain) as u exact − u 1 O(h ) 2 4u − u1 = = 4, hence u exact = 2 2 u exact − u 2 O ( h / 2) 3 σ exact − σ1 O( h )1 = = 2, hence σ exact = 2σ 2 − σ1 σ exact − σ 2 O( h / 2)1 where the subscripts 1 and 2 refer to the first and second (refined) analysis respectively. Hence, an approximate absolute percentage error in the displacement and stress (or strain) is then given by u exact − u 2 σ exact − σ 2 x 100% and x 100% u exact σ exact 6.3.30.2 GNL, MNL Analysis Error Estimation: h- or p- Refinement The mesh should be continuously refined until the variation is of no practical relevance. 993 Structural Engineering Analysis and Design Second Edition 6.3.30.3 Adaptive Analysis in MSC.NASTRAN with p-Elements p-elements are elements that have variable degrees-of-freedom. The user can specify the polynomial order for each element (in the 3 direction Px, Py, and Pz) and the program will generate the degrees-of-freedom required. The pelements are CBEAM, CTRIA, CQUAD, CHEXA, CPENTA and CTETRA. The properties of the p-elements will be specified using the PSOLID, PSHELL, PBEAM, or PBEAML entry. These elements may use either isotropic materials as defined on the MAT1 entry or anisotropic materials as defined on the MAT9 entry. One of the main applications of p-version elements is detailed stress analysis. The p-elements have higher-order polynomials, which provide better representation of complex stress fields. For these complex stress fields, the geometry, loads, and boundary conditions must be represented accurately. This includes modelling fillets instead of sharp corners, distributed loads and constraints instead of point loads and constraints, etc. A more detailed model leads to more detailed results. The accuracy of the analysis is controlled primarily by the polynomial level, not by the element size. Generally the user needs to only use the minimum number of elements necessary to adequately model the geometry, independent of expected result characteristics. Polynomials levels can then be assigned based on areas of the model in which the user is interested, and areas of the model in which the user is not. (Of course the same polynomial level can be assigned everywhere for a minimum of user involvement, but this is not as efficient.) If a more accurate answer is necessary, the polynomial levels can be increased, either manually by the user or automatically by the program, until the answers reach the specified accuracy, without changing the mesh. Adding degrees of freedom until the error decreases to a specified level is known as adaptivity. By adding higher-order polynomials instead of refining the mesh, a faster rate of convergence, and therefore less iteration, can be achieved. In MSC.NASTRAN, p-elements have been added to complement the existing h-elements. The error estimator requires only a single analysis, not the difference between two analyses. For linear elements, it is based on the gridpoint stress discontinuity; for higher polynomial orders, it considers the contribution of the additional terms for the individual edge, face, and body functions. Therefore it provides efficient information because of the directional sensitivity within the elements. The main advantage of implementing p-elements in MSC.NASTRAN is the ability to combine them with the existing h-elements for global/local analysis. The mesh could consist mostly of h-version elements, with p-version elements in the areas of interest. This method of global/local interface is the most accurate, because it provides both stiffness and loads information, rather than transferring just boundary displacements or tractions into the local model. h-version elements still have several advantages. They are better for global behavior, such as loads analysis, where the exact geometry is not used. They are better for strongly singular problems, such as nonlinear problems. Approximations, such as sharp corners, point loads, point constraints, MPC's, etc. may be used. For a given iteration, they tend to have shorter solution times and use less disk space. Finally, h-elements are a very mature technology. Putting both approaches in the same program combines the advantages for general problems. The pelements may be connected directly to the existing h-elements, and continuity is automatically enforced. This provides global/local analysis in a single run. Most general problems have both some global and some local aspects; i.e., regions where h-elements and p-elements, respectively, are appropriate. Therefore the best approach is combined h- and p-adaptivity, with different criteria in different parts of the model. For p-version elements in detailed stress analysis, it is important to use distributed loads. Concentrated forces cause singularities in the stress field, and therefore should be avoided. The PLOAD4 and GRAV entries can also be applied to p-elements. The FORCE entry can be used, but should only be used where the adjacent elements have a fixed p-level and the results are not of interest. As with the loads, it is important to use distributed boundary conditions for p-version elements in detailed stress analysis. Concentrated boundary conditions also cause singularities in the stress field and should be avoided. The current SPC and SPC1 entries can be used, but should only be used to prevent rigid-body motion or used where the adjacent elements have a fixed p-level and the results are not of interest. 994 Structural Engineering Analysis and Design Second Edition Clearly, with p-elements, a different geometry definition is required. In linear elements, only the corner grid definitions are required. In parabolic elements, the corner and mid-side grid definitions are required to map the curvature of the surface. The Bulk Data entries to define the associativity between the finite element model and the geometrical model are the FEEDGE and FEFACE entries for the edges and faces, respectively. Geometrical curves and surfaces are defined by the GMCURV and GMSURF entries. The GMLOAD entry has been defined to apply (non-singular) loads on these geometric surfaces for the p-version elements. The GMSPC and GMBC entries have been defined to apply (non-singular) boundary constraints for the p-version elements. In order for an element to be recognized as a p-version element, it must be assigned the polynomial values in the new PVAL Bulk Data entry, which is referenced in the ADAPT Bulk Data entry. In order for the p-element to be adaptive, the adaptivity parameters must be assigned in the ADAPT entry. The new PVAL Bulk Data entry assigns the polynomial levels for the three directions to a single element or a set of elements, and is referenced in the ADAPT Bulk Data entry. By default, the three directions are along the element edges. If a coordinate system is specified, the polynomial level of each edge is set to a weighted combination of the coordinate directions. There may be multiple PVALs with the same ID; all of the elements do not have to use the same entry. Each p-version element must have a starting, minimum, and maximum PVAL ID; however, these do not need to be unique. Since the polynomial levels can not decrease, the starting and minimum PVAL IDs can be the same. If the starting and maximum PVAL IDs are the same, the element will have a fixed p-level. After the p-value distribution has been defined, all of the values will be resolved to ensure displacement continuity. This includes selecting the highest plevel specified for elements with common edges, decreasing the p-level for p-elements adjacent to h-elements, and increasing the p-level on curved edges to adequately map them. The new ADAPT Bulk Data entry controls the p adaptivity. The ADAPT Bulk Data entry is referenced with the ADAPT Case Control command, and there may only be one unique ADAPT command in the Bulk Data file. The ADAPT entry contains the IDs for the starting, minimum, and maximum p-value distributions and the maximum number of iterations. It also contains the adaptivity parameters, which may be assigned differently to different sets of elements. These sets of elements do not have to correspond with any sets used in the PVAL entries. The adaptivity type may be element-by-element p adaptive, uniform p-adaptive, no change, or list of p-distributions. For each set in the ADAPT entry, the error estimator method, error tolerance, and stress and strain tolerances are specified. If a p-version element is not included in one of the sets, it is not adaptive. For a non-adaptive p-version solution, the ADAPT Bulk Data entry may specify a maximum of one iteration, or may specify an adaptivity type of no change for all the elements. A third way is to use the PSET Bulk Data entries, which have the same format as the PVAL entry, and reference them with the ADAPT Case Control command. Since the p-version analysis may have multiple iterations, the output control must have the capability of differing among the iterations. For this reason, the OUTPUT Bulk Data entry was added. For a given set of elements, the conventional displacements, stresses, and strains, as well as the new element errors and polynomial values, may be printed, plotted, or punched for the given iteration. The OUTPUT entry is referenced by the DATAREC Case Control command. The conventional Case Control commands still apply to all iterations, but the OUTPUT entry has precedence. The p-version elements also tend to be larger than h-version elements, and have higher order distributions of displacements, stresses, and strains. Therefore results only at the grid points are not adequate, especially for most plotting packages, which use linear interpolation. For data recovery, the p-version elements are divided into view-grids and view-elements in order to better visualize the results. The new OUTRCV Bulk Data entry defines the number of view-elements in each element direction and the output coordinate system for the viewgrids and view-elements. The OUTRCV entry is referenced by the OUTRCV Case Control command. The coordinates of the view-grids may be output using the VUGRID Case Control command. When undertaking a h- or p- refinement, it is important to remember to also alter the boundary conditions and constraints i.e. SPCs and RBEs such that the additional h-refined nodes and the p-refined mid-side nodes on the edges and faces of the supports and constraints also participate. 995 Structural Engineering Analysis and Design Second Edition 996 Structural Engineering Analysis and Design Second Edition 6.3.30.4 Stress Discontinuity Error Estimator Stress recovery concepts, namely I. stress recovery at the element Gauss points, then II. subsequent stress extrapolation to the element grids, and III. eventually, the (transformation into global coordinates and) averaging of the elemental stresses to yield the grid point stresses have been covered. Here we shall discuss error estimation based on grid and element stress discontinuities. For discussion purposes, the averaging process used to compute the stress components at the grid points can be represented in the form 6.3.30.4.1 Grid Point Stress Discontinuity An estimate of the probable error in the stress component δg at the grid point is Thus, the probable error in δg is the root mean square error in δei divided by √Ne. The probable error δg provides an estimated error for each of the stress components. It is probably more useful and more desirable to combine these six (in general there are six component stresses) estimated errors into a single representative error measure at each grid point. An approximate root mean square value of the three estimated errors for each of the stress components offers such a representative error measure. where NC is the number of stress components, three for shells and six for solids. Smaller values of δg and ERROR ESTIMATE are usually obtained for elements with vertex stresses, i.e. most elements except CTRIA3 and CQUAD4 with STRESS (CENTER) option. CQUAD4 with STRESS (CORNER) option will usually yield a smaller δg and ERROR ESTIMATE. These seemingly large values of error estimators for CQUAD4 elements are not uncommon occurrences in statistical error measures. For example, the mean and variance have direct analogies in engineering mechanics. The mean is analogous to the centroid of a body and is thus a measure of where the mass is centered. The variance is the second moment about the mean, and it tends to be 997 Structural Engineering Analysis and Design Second Edition small if the majority of the mass is concentrated about the centroid. As the mass is dispersed further from the centroid, the moment of inertia tends to increase. If the mass is concentrated at the centroid (as it might be in some idealized lumped mass models), the moment of inertia becomes zero. Thus, the error estimates for CQUAD4 elements tend toward larger values because the data used to compute the estimators is dispersed relatively far from the mean. For those elements that provide stress data at vertices, the estimators tend toward smaller values because the stress data tends to be concentrated about the mean in well-designed finite element models. You are cautioned that very inaccurate values of these error estimators may occur at the edges of defined SURFACEs and on the faces of defined VOLUMEs. In summary, the error estimators under discussion can, in some cases, be highly inaccurate. Nevertheless, these data are quite useful when interpreted properly. Provided that grid point stresses are requested (printed by GPSTRESS and plotted by STRFIELD, with SURFACE and/or VOLUME definition), grid point stress discontinuities can be requested with GPSDCON = < Set of Surface / Volume IDs >. Note that GPSTRESS, STRFIELD and GPSDCON all reference the same set. Note that stress continuity data is not provided when both plate and solid elements are connected to a grid point that is involved in stress discontinuity calculations. The printed output is presented as follows. 998 Structural Engineering Analysis and Design Second Edition 6.3.30.4.2 Element Stress Discontinuity The root mean square errors for each stress component of an element may be computed from the values of δei that are computed for each of the Ng connected vertex grid points where δei = σe – σgi. This computation is done for each stress component for all of the elements of interest. It is desirable to combine these six (in general there are six stress component) estimated errors into a single representative error estimate for each element. The root mean square value of the stress error estimates for each of the stress components offers such a representative error measure. Provided that grid point stresses are requested (printed by GPSTRESS and plotted by STRFIELD, with SURFACE and/or VOLUME definition), element stress discontinuities can be requested with ELSDCON = < Set of Surface / Volume IDs >. Note that GPSTRESS, STRFIELD and ELSDCON all reference the same set. 999 Structural Engineering Analysis and Design Second Edition 6.3.30.5 Hand Verification: Deriving Stresses From Forces (Axial, Moments, Shear and Torsion) in Beam Elements and Stresses Due to External Loading of General Shell and Solid Continuum 6.3.30.5.1 Beam – Axial Force Axial forces cause uniform longitudinal normal stresses according to σ = F/A (Engineers Axial Theory σ = F/A = Edu/dx). 6.3.30.5.2 Beam – Bending Moment and Shear Force Assuming linear elastic theory and small displacement theory (i.e. that plane sections remain plane and orthogonal to the neutral axis on bending), bending moments cause longitudinal normal bending stresses varying linearly across the section according to σ = My/I (Engineers Bending Theory σ/y = M/I = E/R = Ed2u/dx2), hence zero at the neutral axis and maximum at the flanges. Longitudinal normal stresses σ = My/I Defining x as the longitudinal axis, the general symmetrical bending equation is σ= My Mz y+ z I zz I yy Whenever bending occurs about an unsymmetrical axis, the unsymmetrical bending equation should be used. σ= (M z I yy (I + M y I yz yy I zz − I 2yz ) ) y+ (M z I yz (I + M y I zz yy I zz − I 2yz ) ) z Shear forces cause vertical and complimentary longitudinal horizontal shear stresses varying parabolically across the vertical dimension of the section according to τ = VQ/Ib (Engineers Shear Theory τ = VQ/(Ib) or on average V/(GAs) = Gdu/dx) where b is the width, V is the shear force, I the second moment of area about the neutral axis and Q the first moment of area about the neutral axis of the area away from the point of concern. The shear stress is hence maximum at the neutral axis and is carried primarily by the web. Shear forces also cause horizontal and complimentary longitudinal shear stresses varying linearly in the flange according to τ = VQ/Ib. Vertical and complimentary longitudinal shear stresses τ = VQ/Ib 1000 Structural Engineering Analysis and Design Second Edition Horizontal and complimentary longitudinal shear stresses τ = VQ/Ib The shear deformation expression is often simplified from VQ/(GIb) to V/(GAs) i.e. V/(GKsA). Section 6.4.2.2 gives values of Ks for typical beam sections which could be used to derive averaged (not maximum) shear stresses. 6.3.30.5.3 Circular Closed (Hollow or Solid) Beam – Torsional Moment A member is subjected to torsion from a shear force when it is applied not at its shear center. For a round section (hollow or solid), if plane and parallel cross sections remain plane and parallel, torsion causes complimentary shear stresses (a state of pure shear) to develop at a radius r according to τ = Tr/J (Engineers Torsion Theory τ/r = T/J = Gdφ/dx) where the torsional constant J is equal to the sections polar moment of inertia for this round section. The maximum hence occurs at the outermost radius. 6.3.30.5.4 Non-circular Closed (Hollow) Beam – Torsional Moment That of a thin-walled arbitrary closed cross-section, τ = T / (2Aet) where Ae is the area enclosed by mid thickness. 6.3.30.5.5 Non-circular Open Beam – Torsional Moment The torsional stress distribution for a noncircular section is much more complicated with J often replaced by Kt. Section 6.4.2.1 gives values of Kt for typical beam sections which could be used to derive torsional shear stresses according to τ = function (T, Kt, geometry)26. The expression τ = Tr/Kt CANNOT be used for general non-circular sections. 6.3.30.5.6 Cylinder – Internal and/or External Pressure A capped cylinder subject to internal or external pressure will develop tangential (hoop), radial and longitudinal normal stresses. Denoting pi and po as internal and external pressure, ri and ro as internal and external radii, and r as the general radius, these stresses are σ tan gential = σ radial = p i ri 2 − p o ro 2 − ri 2 ro 2 (p o − p i ) / r 2 2 2 p i ri 2 − p o ro 2 + ri 2 ro 2 (p o − p i ) / r 2 σ longitudin al = 26 ro − ri ro − ri 2 2 p i ri 2 − p o ro 2 ro 2 − ri 2 ROARK, R.J. and YOUNG, W.C. Roark’s Formulas for Stress and Strain 7th Edition. McGraw-Hill, London. 1001 Structural Engineering Analysis and Design Second Edition The tangential and radial stresses are a long way away from the end caps and the longitudinal stress is constant along the length. 6.3.30.5.7 Thin Walled Cylinder – Internal Pressure For a thin-walled cylinder with diameter d, and thickness t less than 1/20 of its radius, with negligible outside pressure, the maximum tangential (positive for tension) and constant longitudinal (positive for tension) normal stresses are p i (d i + t ) 2t pd = i i 4t σ tan gential , max = σ longitudin al whilst the radial normal stress would simply be the internal pressure (negative for compression) on the element on the inside surface of the cylinder and zero on the element on the outside surface. 6.3.30.5.8 Thin Walled Sphere – Internal Pressure For a thin-walled sphere with diameter d and thickness t, the biaxial (in two orthogonal directions) tangential (positive for tension) normal stresses are pd σ tan gential , max = i 2t whilst the radial normal stress would simply be the internal pressure (negative for compression) on the element on the inside surface of the cylinder and zero on the element on the outside surface. 1002 Structural Engineering Analysis and Design Second Edition 6.4 Stiffness Element Cards The basic MSC.NASTRAN element connectivity structure is shown below. ELEMENT CONNECTION CARD GRID PROPERTY CARD (HM: prop collector for scalar and beams and comp collector for shells and solids) MATERIAL CARD (HM: mat collector) Basic MSC.NASTRAN element and property card structure For beams, the element definition and element stress recovery are performed in the element coordinate system. For shells, the element definition and element stress recovery are performed in the element coordinate system by default (but defined by MCID entry on element connection card; 0 for basic projected, > 0 for user projected, < blank > for element coordinate system, > 0.0 and < 360.0 for angled from side n1-n2 of element). For solid elements, the element definition and element stress recovery are performed in the basic coordinate system by default (but defined on CORDM field of PSOLID; 0 for basic, > 0 for user-defined, -1 for element coordinate system). 1003 Structural Engineering Analysis and Design Second Edition 6.4.1 Scalar CELAS Element CELAS element is used to model springs (that provide translational or rotational stiffnesses) connecting single DOFs at two grid points that should be coincident. If one of the grid points is omitted, then the spring is assumed to be grounded (i.e. a grid which is constrained in displacement). As with any scalar element, the CELAS element MUST BE DEFINED as a ZERO LENGTH element (as a scalar element should not have a dimension anyway), and not one with a finite length. Otherwise, any forces applied to the grids by the scalar element WILL INCORRECTLY induce moments on the structure if the direction of the scalar stiffness (and hence force) is not parallel with the finite dimension. If the grids are not coincident, a difference in displacement may be caused by a rigid body rotation. This situation causes forces in springs and a net moment on the structure, i.e. and internal constraint. Internal constraints can be detected when there is a discrepancy between the OLOAD resultants and SPCFORCE resultants. Although the results with internal constraints could be plausible for static linear analysis, they can be terribly incorrect for eigenvalue analysis. For best practice, always utilize rigid elements to add finite length, even if scalar stiffness parallel to dimension, note that CBUSH elements generated internal rigids. Rigid CELAS with CROD (parallel to rigid element) defined on both coincident grids The DOFs connected by the spring are in the coordinate system defined at the grids. It is convenient if the springs are oriented parallel to the Basic System. In general the direction of the scalar stiffness value will not be coincident with a global DOF. This necessitates the definition of a local coordinate system using CORD1R or CORD2R at the grid where the scalar stiffness is required. This system should be specified in Field 7 of both connected GRID cards. In such situations using a CROD element is sometimes easier than using a spring although with CROD elements, coincident nodes cannot be defined. $ BULK DATA CELAS1 EID PID GA DOF C1 GB DOF C2 PELAS PID1 K1 PID2 K2 PID3 K3 CELAS2 EID K GA DOF C1 GB DOF C2 Structural Damping GE PID4 Structural Damping GE S K4 S When you use CELASi elements to represent concentrated springs between two components of translation, the directions of the two components must be coaxial. Even small deviations in direction can induce a significant moment to your model that does not exist in your physical structure. It is recommended that when a CELASi element is used, the locations of the two end points be coincident in order to avoid this type of problem. If the two end points are not coincident, you should consider using a CROD, CBUSH or CBUSH1D element instead. The CELAS element has somewhat been superceded by the CBUSH and CBUSH1D element to avoid problems with the generation of internal constraints. It is worth noting that the equivalent stiffness of springs in parallel is the addition of the individual stiffnesses and the equivalent stiffness of springs in series is the inverse of the addition of the inverse of the individual stiffnesses. The force in CELAS spring element is calculated as F = K(u1-u2), and hence the sign is dependent upon how the element topology is defined, and not on the physical sense of element force, whether tension or compression. This is not the case in other elements such as CROD, CBAR and CBEAM. The output from the ELFORCE (PRINT) request is as follows. For tension U U2 U1 positive 1004 Structural Engineering Analysis and Design Second Edition 6.4.2 6.4.2.1 One-Dimensional Element Cards Axial and Torsional Stiffness CROD, CONROD, CTUBE Elements A CROD element connects two grid points straight and can provide axial and torsional stiffnesses, hence providing stiffness in only two DOFs at either grid. No bending nor shear stiffnesses are provided. Also, CROD elements do not consider torsional inertia in its mass matrix. NSM is the non-structural mass per unit length. For solid circular sections, the torsional constant Kt be equal to the polar moment of inertia, J = ∫r 2 dA = πR4/2. For thin circular tube sections, Kt = J = π(r14-r24)/2. For non-circular sections, the torsional constant is not be the polar moment of area. Equivalent torsional constants Kt for non-circular sections must be used. An approximation to the torsional constant of noncircular thin walled section depends on whether the thin beam section is closed or open. A thin walled closed section such as a SHS (∫ ) will have Kt = 4A e2 / ds / t where Ae is enclosed area by the mid thickness and the integral is carried out over the circumference. A thin walled open section such as an I-, T- or a channel should be treated as a series of rectangles each contributing to Kt = (1/3)(ds)(t3). 1 b  b 4  3 For general rectangles, K t = 1 − 0.63 1 −  b b max . 3  b max  12b 4max  1 b  3 For narrow rectangles (bmax >> 2b), K t = 1 − 0.63  b b max . 3 b max  1 For very narrow rectangles (bmax >> b), K t = b 3 b max . 3 For squares, Kt = 0.1406b4. For equilateral solid triangles, Kt = 3b 4 / 80 1005 Structural Engineering Analysis and Design Second Edition For general cross sections, extruding a solid or shell model into a beam in an FE program and subjecting it to a torsion, the torsional constant K can be found. To do this, from τ/r = T/J = Gdφ/dx it can be deduced that the rotation of a bar in constant (throughout the length of the beam) torsion T is φ = TL/GJ and replacing J with Kt, the torsional constant Kt can be found. Ensure that there is no other deformation (shear, bending, axial) which contribute to the total deformation, otherwise they must be removed. A suitable system will simply be a encastre cantilever (which is thus statically determinate as far as the equivalent beam is concerned) subject to a torsion at the free end. Hence model the complicated model with one end fixed in all DOFs and the other subject to a torsion T. Of course there will be many forms of deformation (be they axial, bending, shear or torsion) in the local elements of the complicated model, but the equivalent beam idealization will only be subject to a constant torsion T. Hence the resulting twist at the free end φ will be the deformation that will be observed in the idealized beam model due to only torsional deformation and φ = TL/GJ can be used to find J (or Kt). $ BULK DATA CROD EID PID GA GB PROD PID MID Area J C NSM The CONROD element defines the axial and torsional stiffness in the connection card itself. $ BULK DATA CONROD EID GA GB MID Area J C NSM The CTUBE element defines the axial and torsional stiffnesses by specifying the outer diameter and the thickness of a circular tube with a PTUBE entry. The element coordinate system is defined by the direction of the two grids. 1006 Structural Engineering Analysis and Design Second Edition A positive force is tensile by definition and the positive torsion is represented by torsion in a direction according to the Right Hand Rotation Rule about the longitudinal axes directed outwards. These elements are useful to define truss elements where there is no bending. The output from the ELFORCE (PRINT) request is as follows. 1007 Structural Engineering Analysis and Design Second Edition 6.4.2.2 CBAR Element A CBAR element is a straight prismatic element and provides axial, torsional, bending stiffness in two perpendicular planes and shear stiffness in two perpendicular planes, hence providing stiffness in all six DOFs on either grid. Note that CBAR elements do not consider torsional inertias. It is derived from classical beam theory (which assumes that plane sections remain plane in deformation). If this is not deemed to be the case, shell or solids should be used. Since, plane sections must remain plane in deformation, torsional stiffening of out of plane crosssectional warping is neglected. Also, since the shear center and neutral axis must coincide, the CBAR element cannot model warping of open sections. NSM is the non-structural mass per unit length. The CBAR element provides exact results for end loads of any kind, i.e. no element loading. Hence, it models linear bending moment variation exactly. Thus its transverse displacement interpolation function is a cubic polynomial since the bending moment is the second derivative of the transverse displacement in linear beam bending theory. Hence, if there are internal point loads in a structural beam member, discretized the member with a number of finite CBAR elements so that at least all the loads occur at the ends of the CBAR elements. This will prove to yield exact results for a static analysis since the displaced shape for sections with a linear variation of bending moment is cubic polynomial. For modal analyses, it is prudent to use a finer mesh as the mode shapes are not cubic polynomials, in fact are not polynomials at all. The element coordinate system is defined by either an orientation vector or an orientation node, both of which defines a plane in which bending with the second moment of area of I1 occurs. Hence, if I1 is the major principal second moment of area, the orientation node will define the minor axis of bending. The element coordinate system is then defined as shown. Some of the connections of the bar element can be removed by pin-flags. Pin flags can be specified for translational degrees-of-freedom (creating sliding joints), or to rotational degrees-of-freedom (creating hinges). Note that the joints created by the pin-flags occur at the ends of the CBAR’ s neutral axis, not at the grid points. This is akin to disconnecting the bar element from its supporting structure and connecting only certain DOFs. Hence, rotational pin-flags is akin to having two coincident nodes at the end of the bar element (one attached to the bar and the other to the supporting structure) with only the translational DOFs constrained between them. The neutral axis may be offset from the grid point, which is akin to attaching a rigid link between the end of the bar to the support. This is useful to model stiffened plates or grid-works. $ BULK DATA CBAR CBAR EID PID GA GB X1 X2 X3 PA PB W1A W2A W3A W1B W2B EID PID GA GB G0 1008 W3B Structural Engineering Analysis and Design Second Edition PBAR PA PB W1A W2A W3A W1B W2B PID MID Area I1 I2 J NSM C1 C2 D1 D2 E1 E2 F1 K1 K2 I12 W3B F2 X1, X2 and X3 define the orientation vector components in the displacement coordinate system of grid G1. The alternate is to define an orientation grid id G0, but this method is not recommended as alterations to the model will cause the definition to defer. PA and PB are the pin-flags. The Wij are the components of the offset vectors in the displacement coordinate system of G1 and G2. The offset is effectively a rigid element from the grid to the element end. If the CBAR is offset from the grid points and the components of orientation vector are entered (i.e. field 6 of the CBAR entry is a real number), then the tail of orientation vector is at end A, not grid point GA. Conversely, if the orientation vector is defined with the use of another grid point G0 (field 6 of the CBAR entry is an integer number), then the orientation vector is defined as the line originating at grid point GA, not end A, and passing through G0. The Ci, Di, Ei and Fi are the stress recovery coefficients for stress estimation using bending σ = My/I and from the axial forces. Non-symmetric beams will have I12 component. In a beam with a symmetric section, the bending properties depend only in I1 and I2 since they correspond to the principal axes. A load in plane 1 or plane 2 will cause a deflection in only plane 1 or 2. When the section is not symmetric, and is loaded in either plane 1 or plane 2, there is a component of deflection orthogonal to the loading. This occurs because the loading is not in the principal planes. In this case, the bending properties depend on I1, I2 and I12. If in this non-symmetric section, the principal planes were found (by Mohr Circle since I is a second order tensor) and the loading was applied in one of these principal planes, then there will be no orthogonal component to the deflection. 1009 Structural Engineering Analysis and Design Second Edition 1010 Structural Engineering Analysis and Design Second Edition 1011 Structural Engineering Analysis and Design Second Edition Ki are the area factors for shear deformation. Shear stress on a beam is given by τ = VQ/Ib. A simplified expression would simply be τ = V/As where the shear area As is obtained by multiplying the shear area factor Ks to the total area. The shear area factors Ki are as follows. Solid Rectangular K1 = K2 = 5/6 Solid Circular K1 = K2 = 7+ CHS I- and T- Beams Major Axis Minor Axis 6 ν2 (1 + ν )2 K1 = K2 = 1/2 K1 = (5.72/6 to 5.81/6) (Aweb / A) K2 = (5/6) (Aflange / A) For those rare structures where the shear deformation is very important it may be necessary to use a more exact value for the area. The following gives formulae for F for the cross-sections shown below noting that 1012 Structural Engineering Analysis and Design Second Edition The shear stiffness of a castellated beam, or of a truss modelled by a single beam element, is significantly less than for the equivalent solid beam and so shear deformations always need to be allowed for, even with slender beams. It is often convenient in a large analysis to represent trusses by beams with shear flexibility. The axial stiffnesses, EA, of the chords of a truss determine the bending stiffness, whereas the axial stiffnesses of bracing members, or the flexural stiffnesses, EI, of all members, control the shear stiffness. For all trusses and frames with parallel chords of area AF and centroids separated by b, the flexural stiffness EΙ = EAF.b2/2. The shear stiffnesses and shear area factors for trusses and for Vierendeel frames are presented. 1013 Structural Engineering Analysis and Design Second Edition 1014 Structural Engineering Analysis and Design Second Edition If the shear stiffnesses of the members and joints are also considered, then the expressions for Vierendeel frames becomes where S is the rotational stiffness of the joint, and KF and KB are the shear area factors associated with AF and AB respectively and w and h are defined on the joint figure below. For a Vierendeel frame comprising flanged sections with a common web thickness, much of the shear flexibility results from joint deformation. For the joint shown, S, KFAF and KBAB are given by: 1015 Structural Engineering Analysis and Design Second Edition It should be noted that although a frame analysis would not normally include joint deformations, it would include the shear deformations between the face of the perpendicular members and their centre lines. If the above value of K is rewritten as Whether such a model over or under estimates the shear deformations depends on the last term of the denominator and hence the ratios w/a and h/b. For general cross sections, extruding a solid or shell model into a beam in an FE program and subjecting it to a shear force, the shear area can be found. To do this, from τ = V/As = Gdu/dx it can be deduced that the shear deflection of a beam in constant (throughout the length of the beam) shear V is u = VL/(GAs), and hence the shear area As can be found. Ensure that there is no other deformation (bending, axial, torsion) which contribute to the total deformation, otherwise they must be removed. A suitable system will simply be a encastre cantilever (which is thus statically determinate as far as the equivalent beam is concerned) subject to a concentrated force at the free end. Hence model the complicated model with one end fixed in all DOFs and the other subject to a force V. Of course there will be many forms of deformation (be they axial, bending, shear or torsion) in the local elements of the complicated model, but the equivalent beam idealization will only be subject to a constant shear force V and a linearly varying bending moment. Hence the resulting deflection at the free end will be the deformation that will be observed in the idealized beam model due to both shear and bending deformations, the cantilever will not be subject to any axial nor torsional forces. The component of the deflection which is due to bending deformation must be known. This must be calculated from classical methods, i.e. ubending = VL3/(3EI) where I is calculated from a closed form formula. The remaining deflection after ubending is subtracted is the shear deflection which can then be used to back calculate the shear area As from u = VL/(GAs). The PBARL is an alternative method of defining the PBAR entry. The PBARL Bulk Data entry allows you to input cross section types along with their characteristic dimensions. You can choose from19 different cross section shapes. These shapes are as follows: ROD, TUBE, I, CHAN (channel), T, BOX, BAR (rectangle), CROSS, H, T1, I1, CHAN1, Z, CHAN2, T2, BOX1, HEXA (hexagon), HAT (hat section), and HAT1. Because of the knowledge of the section type, the stress recovery points are automatically defined. 1016 Structural Engineering Analysis and Design Second Edition $ BULK DATA PBARL PID MID DIM1 DIM2 Group (MSCBML0) DIM3 DIM9 etc.. NSM TYPE DIM4 The output from the ELFORCE (PRINT) request is as follows. 1017 DIM5 DIM6 DIM7 DIM8 Structural Engineering Analysis and Design Second Edition 6.4.2.3 CBEAM Element A CBEAM element includes the CBAR element capabilities and separate neutral axis and axis of shear centers, effect of cross-sectional warping on torsional stiffness (as is important in the case of open sections), cross-sectional properties specified on both ends and interior point (tapered element), effect of taper on traverse shear stiffness (shear relief), separate axis for the center of non-structural mass and torsional inertias are included i.e. can be offset from shear center (for dynamic analyses) and also has nonzero rotational mass moment of inertia about its neutral axis. The CBEAM element can be loaded at interior points by means of the PLOAD1 card. But again, the CBEAM element is only exact if loads are applied at its ends, i.e. it models a linear bending moment distribution. NSM is the non-structural mass per unit length. The element x-axis is along the shear center unlike CBAR where it is along the neutral axis. $ BULK DATA CBEAM PBEAM EID PID GA GB X1 X2 X3 PA PB W1A W2A W3A W1B W2B W3B SA SB PID MID A(A) I1(A) I2(A) I12(A) J(A) NSM(A) C1(A) C2(A) D1(A) D2(A) E1(A) E2(A) F1(A) F2(A) K1 K2 I12 … … … … … … … … S0 X/XB A I1 I2 I12 J NSM C1 C2 D1 D2 E1 E2 F1 F2 … … … … … … … … K1 K2 S1 S2 NSI(A) NSI(B) CW(A) CW(B) M1(A) M2(A) M1(B) M2(B) N1(A) N2(A) N1(B) N2(B) For the CBAR element, the element stiffness matrix is generated directly from the input data. For instance, if I1 for a CBAR element is zero, then the corresponding element stiffness matrix term is null, which is not necessarily a problem. On the other hand, the CBEAM element uses the input data to generate an element flexibility matrix, which must be inverted to produce the element stiffness matrix. Therefore, positive values for A, I1, and I2 must be entered. One difference between the CBAR element and the CBEAM element, that is not obvious, is the default values used for the transverse shear flexibility. For the CBAR element, the default values for K1 and K2 are infinite, which is equivalent to zero transverse shear flexibility. For the CBEAM element, the default values for K1 and K2 are both 1.0, which includes the effect of transverse shear in the elements. If you want to set the transverse shear flexibility to zero, which is the same as the CBAR element, use a value of 0.0 for K1 and K2. Analogous to PBARL, PBEAML can be used to generate the section properties from the dimensions. 1018 Structural Engineering Analysis and Design Second Edition The output from the ELFORCE (PRINT) request is as follows. 6.4.2.4 CBEND Element A CBEND element is a circular arc between 2 grids with extensional, torsional, bending stiffness in two perpendicular planes and shear stiffness in two perpendicular planes. The PBEND card has two alternate forms, corresponding to a curved beam of arbitrary cross-section or a curved pipe (tube). The curved beam has its principal bending axes parallel and perpendicular to the plane of the element, the geometric centre of the element may be offset in two perpendicular directions, the offset of the neutral axis from the geometric centre due to curvature is calculated automatically. For the curved beam form of the element a user override is possible. For the curved pipe form, the effect of internal pressure on stiffness and stress can be accounted for. Axial stresses can be output at four cross-sectional points at each end of the element. Forces and moments are output at both ends. Distributed loads may be applied along the element using the PLOAD1 card. NSM is the non-structural mass per unit length. The output from the ELFORCE (PRINT) request is as follows. 1019 Structural Engineering Analysis and Design Second Edition 6.4.3 Two-Dimensional Element Cards For linear analysis, shells assume the classical assumptions of this plate behavior, i.e. the thickness must be much smaller than the other dimensions, the deflection at the mid-surface must be small compared to its thickness and the mid-surface remains unstrained during bending by lateral loads. The force, moment and stress are output. The Element Coordinate System is defined implicitly by the locations and order of the connected grid points in the Element Coordinate System. The element x-direction is defined by a vector from the first to the second grid point defined in the connectivity card. The element y-direction is perpendicular to the x-direction, and lies in the plane of the element. The element z-direction is defined by the right-hand rule. It is not really necessary to orient the X- and Y- axes of the elements in a common fashion so long as the element stresses are transformed into global coordinates in the post-processor. But it is always necessary to orient the Z-axis of the elements consistently as the stresses at the top and bottom surfaces are viewed separately. Forces and moments are output at the element center whilst stresses are output at distances Z1 and Z2 from the centroid surface. If Zi = ½ thickness (by default), then the stresses are output at the surfaces. 6.4.3.1 Transverse Bending, Transverse Shear and In-Plane Membrane (Plane Stress or Plane Strain) CQUAD4, CQUAD8, CTRIA3, CTRIA6 Elements In general, the quadrilateral elements CQUAD4 and CQUAD8 should be preferred over the triangular elements CTRIA3 and CTRIA6, which are stiffer particularly for membrane strain. The latter are mainly useful to model portions of a structure when quadrilateral elements are impractical. Shell elements have 5 DOFs at each grid point, i.e. they do not have in plane rotational freedoms. Variable thickness can be defined, hence tapering is possible. For CTRIA6 and CQUAD8, the mid-side grid point need not be located on a straight line joining the adjacent corner points (because of the nature of isoparametric elements), hence these elements can model curved surfaces. The shell elements have the capabilities of membrane stiffness, transverse bending stiffness and transverse shear stiffness. The membrane stiffness can be calculated using either the plane stress (default) or plane strain theories. Any of these capabilities may be omitted by the user. The elements CQUAD4, CQUAD8, CTRIA3 and CTRIA6 employ either the PSHELL or PCOMP property cards. Both the PSHELL and PCOMP cards can refer to either MAT1, MAT2 or MAT8. (Note that PSOLID cards refer to MAT1 or MAT9). The PSHELL card is described. $ BULK DATA PSHELL PID MID1 T Z1 Z2 MID4 MID2 12I/T3 MID3 TS/T NSM MID1 - Material for membrane stiffness. MID2 - Material for bending stiffness. MID3 - Material for transverse shear stiffness (thick plate theory for thicker shells) MID4 - Material for coupling between membrane and bending deformation to model offsets. 12I/T3 is the bending stiffness parameter, by default 1.0 TS/T is the transverse shear thickness divided by the membrane thickness, by default .833333 NSM is the non-structural mass per unit area For solid homogenous plates, the default values of 12I/T3 and TS/T are correct. To obtain pure membrane behaviour only the MID1 should be specified; To obtain pure plate bending behaviour only the MID2 and MID3 fields should be specified. In reality, transverse load is resisted by both bending and membrane action, the latter when the geometry is curved or becomes curved as the nonlinear analysis progresses. Membrane action is the tension that occurs in the plane of the plate once some deformation has taken place, and this acts to resist the transverse force. For thin shells, membrane action is stiff compared to bending. Finally, transverse shear flexibility should be omitted only for comparison with academic solutions; Including the transverse shear flexibility always 1020 Structural Engineering Analysis and Design Second Edition gives a better answer for real-world structures. An element with shear flexibility will deflect more than an element without shear flexibility, hence the term shear flexibility instead of shear stiffness. The thicker the plate, the more significant is the contribution from the shear flexibility term, analogous to short deep beams. But for thin or curved surfaces, it is advisable not to use MID3. The MID4 is simulating a similar effect to having an offset i.e. if you apply a tension (membrane load) it will cause bending deflections if you have this material set. It is rarely used but can be automatically generated on an unbalanced PCOMP entry. This has nothing to do with differential stiffness, which is accounted for nevertheless (with appropriate elements). Other methods of modelling plate offsets are by using ZOFFS on the element card or by using explicit rigid RBAR elements. Of the three methods MID4, ZOFFS and RBAR, the recommended approach is by using ZOFFS. The PCOMP property card is used for modelling a composite material consisting of layers. This information is used internally within NASTRAN to compute equivalent PSHELL cards. 6.4.3.1.1 CQUAD4 Element CQUAD4 element is a modified isoparametric element. Its membrane part uses reduced order integration for inplane shear. Its bending part gives nearly exact results when the curvature varies linearly over the surface of the element. This element is the most commonly used element in NASTRAN. CQUAD4 are better for doubly-curved shells such as spheres. It is a robust element and behaves well when its shape is irregular. For example good results have been obtained with skew angles up to 45 degrees. There is no aspect ratio limit. The corner points are not required to lie in the same plane. It is recommended to avoid warping angles larger than 10 degrees. $ BULK DATA CQUAD4 EID PID G1 G2 G3 G4 T1 T2 T3 T4 THETA OR MCID ZOFFS Ti represents the shell thickness at the 4 corners, which can be omitted, in which case they will be set to the thickness defined in the property entry card. ZOFFS is used to model the plate offset. A positive ZOFFS implies that the element reference plane is offset a distance ZOFFS from the grid points along the positive z-axis of the element coordinate system. Naturally, MID1 and MID2 must be specified if offsets are used. It is important to note that the forces generated for the elements are forces per unit length. A common error for new users is to assume that the force shown in the output is the total force acting on the element—it is not! It is the force per unit length. 1021 Structural Engineering Analysis and Design Second Edition 6.4.3.1.2 CQUAD8 Element The CQUAD8 is a modified isoparametric element with four corner grid points and four edge grid points. Compared with the CQUAD4 element, the CQUAD8 element usually provides greater accuracy at the same cost for flat plates and for singly-curved shells (such as a cylinder). The CQUAD4 however tends to perform better for doubly-curved shells (such as a sphere). For modelling cylindrical surfaces, the CQUAD8 should not sweep more than 30 degrees of the surface. CQUAD8 for mesh transition is not recommended. Deleting mid-side nodes is NOT recommended. For the CQUAD8 elements, if mid-side nodes are present, they should be located within the middle third of the edge. If a mid-side node is located at one-fourth the distance of the edge as measured from either corner node on the edge, the internal strain field becomes singular at the corners of the element. For best results, it is recommended that the mid-side node be located as close to the center of the edge as possible. If mid-side nodes are desired, the general recommendation is to include all of them. A CQUAD8 element with mid-side nodes deleted is excessively stiff and therefore is inferior to a CQUAD4 element. $ BULK DATA CQUAD8 EID PID G1 G2 G3 G4 G7 G8 T1 T2 T3 T4 G5 THETA OR MCID G6 ZOFFS QUAD8 is better than QUAD4 when there is in-plane bending because QUAD8 can curve because of the existence of mid-side nodes and its isoparametric formulation whilst the QUAD4 is straight at its edges, exhibiting shear locking behavior. QUAD8 is better than QUAD4 when there is out-of-plane bending because the stress recovery is linear (σx in x) in QUAD8 whilst constant in QUAD4. 6.4.3.1.3 CTRIA3 Element CTRIA3 element is a constant strain, constant curvature triangle. CTRIA3 elements have constant membrane stresses. They are therefore not suitable for modelling areas with stress gradients (for example in the web of an Ibeam) and SHOULD BE MINIMIZED. Quadrilateral elements (CQUAD4, CQUAD8) or CTRIA6 triangles are preferable. The primary application is to model portions of the structure where quadrilaterals are impractical, such as the center of a circular plate. Avoid using CTRIA3 in locations where the membrane stresses are changing rapidly, for example, in the web of an I-beam. Since CTRIA3 has constant membrane stresses, a large number of them may be needed to obtain acceptable accuracy. It is better to use quadrilateral elements or CTRIA6 elements. In fact, two CTRIA3 is not better than one QUAD4. To illustrate this, consider the membrane CQUAD4, which has 8 DOFs, i.e. capable of representing 8 independent deformation states, 3 of which are rigid body modes, leaving 5 independent stress-inducing deformation states. Contrast with the membrane CTRIA3, which has 6 DOFs, i.e. capable of representing 6 independent deformation states, 3 of which are rigid body modes, leaving 3 independent stress-inducing deformation states. Hence, two deformation states cannot be represented accurately by the CTRIA3 that can be by the CQUAD4. $ BULK DATA CTRIA3 EID PID G1 G2 G3 T1 T2 T3 THETA OR MCID ZOFFS Ti represents the shell thickness at the 4 corners, which can be omitted, in which case they will be set to the thickness defined in the property entry card. 6.4.3.1.4 CTRIA6 Element CTRIA6 is a linear strain, linear curvature triangle with 3 corner nodes and 3 mid-side nodes. It is used in a similar way to CTRIA3, in areas where QUAD elements are unsuitable, in meshes with other elements having edge grids. 1022 Structural Engineering Analysis and Design Second Edition 6.4.3.2 In-Plane Shear and Extension CSHEAR Elements The CSHEAR element is a quadrilateral with 4 grid points that supports in-plane shear force only. It is used in the analysis of thin reinforced panels, especially if the panels are curved or buckled. The panels are then modeled by CROD elements carrying extensional loads and CSHEAR elements carrying in-plane shear. The CSHEAR element can also carry extensional force between adjacent grid points using the optional parameters F1 and F2 on the PSHEAR card. This offers an efficient way to model the stiffness of the panel for extensional loads. Typically you use the CSHEAR element in situations where the bending stiffness and axial membrane stiffness of the plate is negligible. The use of CQUAD4 element in such situations results in an overly stiff model. The most important application of the CSHEAR element is in the analysis of thin reinforced plates and shells, such as thin aircraft skin panels. In such applications, reinforcing rods (or beams) carry the extensional load, and the CSHEAR element carries the in-plane shear. This is particularly true if the real panel is buckled or if it is curved. Do not use plate or shell elements (CQUADi, CTRIAi) in stiffened shell structures with very thin panels that can buckle. Shear panels (CSHEAR) should be used in this case or in any situation where direct stresses cannot be supported, such as in a very thin curved panel. $ BULK DATA CSHEAR EID PID G1 G2 G3 G4 PSHEAR PID MID T NSM F1 F2 The optional parameters F1 and F2 on the PSHEAR entry are useful in representing an effective stiffness of the panel for extensional loads by means of equivalent rods on the perimeter of the element. 6.4.3.3 CRACK2D The CRAC2D element is used to model surfaces with a discontinuity due to a crack. 1023 Structural Engineering Analysis and Design Second Edition 6.4.4 Three-Dimensional Element Cards Solid elements connect only translational DOFs at grid points. $ BULK DATA PSOLID PID MID CORDM IN STRESS ISOP FCNT CORDM is the material coordinate system IN is the integration network STRESS is the location for stress output ISOP is the integration scheme FCNT is the fluid element flag, SMECH for structural element and PFLUID for fluid element. Unlike plate and shell elements where stress components are always recorded in the element coordinate system, the stresses for the HEXA and PENTA elements are recorded in the material coordinate system. The user has a several ways of defining the material coordinate system specified on Field 4, either the Basic Coordinate System (0 or blank as default), the Element Coordinate System (-1), or a Local Coordinate System (Integer > 0). By default, the stress output for the solid elements is at the center and at each of the corner points. For CHEXA and CPENTA, if no mid-side nodes are used, you may request the stress output at the Gauss points instead of the corner points by setting Field 6 of the PSOLID entry to “GAUSS” or 1. Gauss point output is available for the CTETRA element with or without mid-side nodes. The default integration schemes may be overridden with Field 5 and Field 7 of the PSOLID entry. In general, it is recommended that you use the default value. An override of the default values is available if you are familiar with element theory and have a particular modelling need; otherwise, use the defaults. 1024 Structural Engineering Analysis and Design Second Edition 6.4.4.1 CHEXA8 or CHEXA20 Element The six-faced CHEXA element has 8 corner nodes forming a rectangular brick shaped element. If mid-side nodes are specified, then there will be an additional 12 grids. This element is more recommended than other degenerate solid elements. Its performance degrades when subjected to prominent bending. The mid-side grids G9 to G20 are optional. Any or all of them may be deleted, but not recommended. The equations are modified to take into account the available grids. Of course, the corner grids cannot be omitted. As in the case of plate elements, if mid-side nodes are present for the solid elements, they should be located as close to the center of the edge as possible. $ BULK DATA CHEXA 6.4.4.2 EID PID G1 G2 G3 G4 G5 G6 G7 G8 G9 G10 G11 G12 G13 G14 G15 G16 G17 G18 G19 G20 CPENTA6 or CPENTA15 Element The five-faced CPENTA element has 6 corner grids and has 9 available mid-side edge grids, forming a wedge shape. It is commonly used to model transitions from solids to shells. The triangular faces should be on the exposed faces of the shells, to avoid excessive stiffness. Any or all of the mid-side grids may be omitted, but is not recommended. $ BULK DATA CPENTA EID PID G1 G2 G3 G4 G5 G6 G7 G8 G9 G10 G11 G12 G13 G14 G15 6.4.4.3 CTETRA4 or CTETRA10 Element The four-faced CTETRA is a quadratic (linear strain) isoparametric solid element with 4 corner grids and 6 available mid-side grid points. A linear (constant strain) CTETRA may be obtained by omitting the edge grid points. Partial omission of edge grid points is allowed, but is not recommended. The recommended application of the CTETRA element is to fill in odd-shaped holes in meshes made with CHEXA and CPENTA elements. If large portions of the model must be modeled using CTETRA elements, then a very fine mesh density is recommended in regions of steep stress gradients. If you use edge nodes, it is recommended that you include all six nodes. The accuracy of the element degrades if some but not all of the edge grid points are used. In bending situations, two or more tetrahedrons are required through the wall thickness to capture behaviour. It is a good modelling practice to keep the use of CTETRA4 TO A MINIMUM, especially in the areas of high stress. CTETRA10 should be used as the standard TETRA element, even before h-refinement is undertaken as CTETRA4 is overly stiff as it is a constant strain element. Studies show that properly converged second order CTETRA10 can provide the same accuracy as a linear brick element. CTETRA has the advantage of being very easy to mesh with an automated mesh generator and is the norm for CFD type applications. A skin of TRIAs are generated with an automated mesh generator on defined surface geometry, then the tetra mesh is employed to fill the volume. The skin can be remained to act for stress recovery purposes on the surface of the component where the stress is most likely to be the highest. Note that the thickness of the skin is usually in the order of around 0.01mm for standard components and connections of 1m nominal dimensions say. 6.4.4.4 CRACK3D The CRAC3D element is used to model volumes with a discontinuity due to a crack. 1025 Structural Engineering Analysis and Design Second Edition 6.5 Mass Element Cards The CMASS1 (with PMASS) and CMASS2 elements define a scalar mass element between two grid points (and across particular DOF pairs in the CD displacement coordinate system of the grid point). The grid IDs G1 and G2 must be distinct, however a zero or blank field will indicate a grounded terminal. $ BULK DATA CMASS1 EID PID PMASS PID1 M1 Grid ID G1 PID2 DOF C1 M2 Grid ID G2 PID3 DOF C2 M3 PID4 M4 $ BULK DATA CMASS2 EID M Grid ID G1 DOF C1 Grid ID G2 DOF C2 The CONM1 element allows input of a fully coupled 6 x 6 mass matrix. Half the terms are defined and symmetry is assumed. $ BULK DATA CONM1 M33 Grid ID M41 M54 M55 EID CID M11 M21 M22 M31 M32 M42 M43 M44 M51 M52 M53 M61 M62 M63 M64 M65 M66 The CONM2 element allows the specification of a concentrated mass at a grid point. This element also allows the definition of a center of gravity offset from the grid point and moments and products of inertia about the center of gravity. $ BULK DATA CONM2 EID I11 Grid ID I21 CID M X1 X2 I22 I31 I32 I33 X3 The mass matrix [M] is automatically computed from (i) (ii) (iii) the mass density (mass per unit volume) in the property cards the non-structural mass (mass/length or mass/area) in the property cards concentrated mass elements The mass matrix [M] is obtained by either the lumped mass method or the coupled mass method (based on the classical consistent mass method). The lumped mass model contains uncoupled components of translational mass and uncoupled components of rotational or torsional inertia components. The lumped mass model thus generates diagonal mass matrices. The coupled mass method on the other hand contains coupled components of mass between translational DOFs and coupled components of inertia between rotational DOFs, but no coupling between translational and rotational DOFs. The coupled mass matrix is thus not diagonal. It formulates the mass matrix by a procedure similar to the formulation of the stiffness matrix by applying unit accelerations at successive nodal freedoms and investigating the force generated at all the freedoms. Although the coupled mass method is more accurate, the lumped mass method is generally preferred for its computational speed. Coupled mass formulation is especially more accurate to model high frequency modes. To specify coupled mass rather than the default lumped mass formulation, 1026 Structural Engineering Analysis and Design Second Edition $ BULK DATA PARAM, COUPMASS, 1 The dynamic mass often includes the medium surrounding the structure. For instance, in the analysis of offshore gravity platforms, some degree of the mass of the water surrounding the shafts must be included within the mass. Noting that the mass acts in 3 translational orthogonal directions (likewise inertia acts about 3 orthogonal axes), it is essential that the correct component be modeled. The added mass on the shafts is a horizontal mass component whilst the added mass on the base of the gravity base structure is a vertical mass component. The inclusion of added masses on the dynamic model also means that a uniform global acceleration applied to all parts of the structure to model gravitational force cannot be employed, as the added mass will incorrectly increase the weight of the structure. Instead, the gravitational force must be modeled using explicit nodal loads or more accurately, gravitational accelerations applied to a set of masses that excludes the added masses. Another important consideration when modelling non-structural mass is that if rigid links are used to model the center of gravity of the non-structural mass from the structure, then a coupled mass formulation (kinematically equivalent mass matrix) must be used. This is because if lumped mass formulation is used, the rigid links simply will transfer the non-structural mass onto the structure, and hence effectively not incorporating the offset. This will cause significant errors in the lowest frequencies 27. 27 NAFEMS. A Finite Element Primer. NAFEMS Ltd., Great Britain, 1992. 1027 Structural Engineering Analysis and Design Second Edition 6.6 6.6.1 Damping Element Cards Viscous Damping Elements CDAMP and CVISC The CDAMP1 (with PDAMP) and CDAMP2 elements define a scalar damping between two grid points (and across particular DOF pairs in the CD displacement coordinate system of the grid point). The damping constant is expressed in units of force/velocity. The grid ids G1 and G2 must be distinct, however a zero or blank field will indicate a grounded terminal. In general the direction of the scalar viscous damping will not be coincident with a global DOF. This necessitates the definition of a local coordinate system using CORD1R or CORD2R at the grids (and defined on Field 7 of the two GRID entries) where the scalar viscous damping is required. As with any scalar element, the CDAMP element MUST BE DEFINED as a ZERO LENGTH element (as a scalar element should not have a dimension anyway), and not one with a finite length in order to avoid internal constraints. To this end, the CDAMP element has been somewhat superceded by the CBUSH or CBUSH1D element. $ BULK DATA CDAMP1 EID PID PDAMP PID1 C1 Grid ID G1 PID2 Grid ID G2 PID3 DOF C1 C2 DOF C2 C3 PID4 C4 $ BULK DATA CDAMP2 EID C Grid ID G1 Grid ID G2 DOF C1 DOF C2 The CVISC element is used to define a viscous damping between two grid points in the direction defined by the vector joining the grids and has an associated PVISC card to define the translational CE and rotational CR viscous damping properties. The grid ids G1 and G2 must be distinct. The CVISC element has been somewhat superceded by the CBUSH or CBUSH1D element. $ BULK DATA CVISC EID PID PVISC PID1 CE1 6.6.2 Grid ID G1 CR1 Grid ID G2 PID2 CE2 CR2 Structural Damping Elements Elemental structural damping is defined as follows. If the model consists of a single material, such as a casting, then only one damping value is needed in which case the PARAM, G can be used $ BULK DATA PARAM, G, < Damping constant > The other way of specifying structural damping is to use GE in the MAT1 card enabling different values to be used for the various components of the model. Structural damping can also be specified using CELAS or CBUSH. 1028 Structural Engineering Analysis and Design Second Edition 6.7 General Nonlinear Excitation Frequency Dependent Spring And Linear Excitation Frequency Dependent Damper CBUSH (PBUSH and PBUSHT) Element Note that the CELASi and CDAMPi elements are non-metric elements. This means that grid point geometry is not used when assembling them into the system stiffness matrix. They will always produce a 2 by 2 matrix, regardless of offsets, coordinate systems, or other modelling details. This can result in internal constraints in the element, which in turn leads to constraint forces to ground that do not appear in the SPC forces. An internal constraint means that the element is not in equilibrium. The effect of internal constraints can be investigated by checking the applied load resultant (OLOAD RESULTANT) and the reaction resultant (SPCFORCE RESULTANT), a discrepancy indicating the existence of internal constraints. The CBUSH element can be thought of as the modern replacement for the CELASi and CDAMPi scalar elements. It is a metric element, and will properly account for offsets, coordinate systems, and any other modelling data. It is always in equilibrium. It is recommended that all scalar elements in models be replaced with CBUSH elements, especially if the input file is passed onto a different modeller. If the new modeller modifies the grid point geometry the CBUSH element will still be in equilibrium. This may not be true for scalar elements. Must NOT use local coordinate systems on GRIDs with CBUSH. The CBUSH element requires the definition of a local coordinate system in itself. The element force is given by f e = k (f , u )u + c(f )u&+ iG E (f ) ku where f is the excitation frequency. Frequency dependent stiffness and damper properties are applicable only to forced frequency response analyses SOL 108, SOL 111 and SOL 200. Nonlinear spring properties are only applicable to SOL 106 and SOL 129. Note however that the CBUSH element is not geometrically nonlinear. CBUSH is the recommended element enabling up to 6 uncoupled stiffness and damping values to be inputted. PBUSH provides nominal values and a PBUSHT (with the same ID as a PBUSH card) provides the frequency dependency and nonlinear characteristics. The third node G0, the orientation vector X1, X2 and X3 or the user defined coordinate system CID defines the element coordinate system. Note that the stiffness and damping values are defined at the elastomer center of elasticity, from which the properties are transferred to the grid nodes using rigid element equations. The output from the ELFORCE (PRINT) request (in the element coordinate system) is as follows. 1029 Structural Engineering Analysis and Design Second Edition 6.8 One Dimensional Nonlinear Spring And Nonlinear Damper CBUSH1D (PBUSH1D) Element The CBUSH1D element is a 1D version of CBUSH but with added features. It is materially and geometrically nonlinear (for stiffness and damping) for SOL 106 and SOL 129. The element force is given by f e = c(u )sign (u&)u&EXPV + k ( u )u + c(u&)u& 1030 Structural Engineering Analysis and Design Second Edition 6.9 6.9.1 Material Cards Linear, Elastic, Isotropic Material Card for 1-D, 2-D and 3-D Elements MAT1 The user needs to specify in the MAT1 card 2 of the 3 elastic constants: elastic modulus E, shear modulus G and Poisson’ s ratio NU. The value of the third constant is calculated by NASTRAN using G = E/[2(1+ν)]. Note that specifying all 3 constants can give incorrect results. $ BULK DATA MAT1 MID E G NU ST SC SS MCSID RHO A TREF GE ST, SC, SS MCSID RHO A E NU CROD, CBAR, CBEAM Extension and bending N/A CQUAD4, CQUAD8, CTRIA3, CTRIA6 CSHEAR CHEXA, CPENTA, CTETRA Concrete Short Term Concrete Long Term Aluminium 6.9.2 GE density thermal expansion coefficient reference temperature for the calculation of thermal loads structural damping coefficient stress limits for tension, compression and shear used only to compute margins of safety in certain elements material coordinate system id Element Steel TREF G Torsion and transverse shear Membrane and bending Transverse shear N/A Shear All terms N/A E (N/m2) ρ (kg/m3) ν Thermal Expansion (Strain/°C) 2.05E11 7850 0.3 1.2E-5 2.8E10 2400 0.2 1.0E-5 1.4E10 2400 0.2 1.0E-5 7.0E10 2710 0.34 2.3E-5 Modelling of concrete as a linear elastic material assumes that the concrete does not crack. The cracking of concrete leads to a redistribution of load. Since the cracking occurs at very low strains, concrete is a highly nonlinear material. In linear analyses, usually a short-term high stiffness concrete and long-term low stiffness concrete stiffness is assumed in separate analyses to bound the results. Linear, Elastic, Anisotropic Elastic Material for Shell MAT2 and Solid Elements MAT9 Anisotropic refers to properties that differ in two or more directions. 6.9.3 Linear, Elastic, Orthotropic Elastic Material for Shell Elements MAT8 and Solid Elements MAT9 Orthotropic refers to a specific type of anisotropy in which planes of extreme values are orthogonal. 1031 Structural Engineering Analysis and Design Second Edition 6.10 Rigid Element Cards Rigid elements are equations of motion connecting DOFs. They therefore do not have physical properties such as cross-section, stiffness or mass. RROD RBAR RTRPLT RBE1 A pin-ended rod which is rigid in extension, i.e. 1 constraint equation A rigid bar with six DOFs at each end, i.e. 6 constraint equations A rigid triangular plate with six DOFs at each vertex, i.e. 12 constraint equations A rigid element connected to an arbitrary number of grid points. The independent and dependent DOFs can be arbitrarily selected by the user. A rigid element connected to an arbitrary number of grid points. The independent DOFs are the six components of motion at a single grid point. The dependent DOFs at the other grid points all have the same component numbers. RBE2 $ BULK DATA RBE2 RBAR EID GN CM GM1 GM6 GM7 GM8 …etc… EID GNA GMB CNA GM2 GM3 GM4 CNB CMA CMB GM5 GN-independent grid; GM-dependent grids; CN-independent grid components; CM-dependent grid components; Note that a dependent DOF in one element cannot also be a dependent DOF in another rigid element since this will produce conflicting equations of motion. The dependent DOF should also have no SPC specified to it. Note however that an independent DOF can be a dependent DOF in another rigid element. Rigid elements are used to I. model connections such as spot welds, II. define hinges or sliding joints, III. distribute loads, IV. connect dissimilar elements such as solids to shells V. model stiffeners on plates; the stiffener can be a CBAR element offset by rigid elements from a shell structure to a distance equal to half the thickness of the stiffener VI. replace very stiff elements, which will produce numerical ill conditioning. Rigid elements, however, should be used with great care. Rigid elements can transfer large loads, but since they are not real elements they do not provide load or stress output. 1032 Structural Engineering Analysis and Design Second Edition Rigid element and MPC grid point forces are requested with MPCFORCES (PRINT, PLOT). Note that akin to GPFORCE, MPCFORCES output the force acting on the grid point, NOT ON THE ELEMENT. In fact, MPCFORCES is the resultant force on the grid point from all adjoining rigid or MPC elements. This is clearly not very useful unless there is only one MPC on the grid, so that the MPCFORCES will be the forces acting on the grid due to ONLY that particular MPC. In that case, we can establish the force within the MPC by switching the directions of the forces as illustrated below. MPCFORCES MPC in Tension MPCFORCES This is very much akin to GPFORCES (in the sense that it is the force on the grid not on the element(s)), hence the reason for omitting forces from rigid or MPC elements from GPFORCE output. In the situation where there are many MPC elements connecting into a grid, the use of a stiff CELAS or CBUSH is necessary to find out the force going through an MPC element. The output from MPCFORCEs is the summation of all MPC-related forces at each GRID point. If only R-elements and MPCs are used to connect a point to the model, NASTRAN will provide 0.0 as the MPCFORCE at that GRID. This may be misleading, as the output does not provide forces for each MPC and Relement separately, rather it provides only the summation of all MPC and R-element forces at the GRID point. For example, if the following model of a beam with a 100.0 unit axial force is used, 100 x------x------x------x RBAR x RBAR x------x------x 100.0 1 2 3 4 5 6 7 8 the MPCFORCE at GRID 5 will show as 0.0, even although each of the connected RBAR elements has an axial force of 100.0 units. If you replace one of the RBARs by a CBUSH element, the MPC-forces will now show the components from the remaining RBAR (100.0 units), which are equal and opposite to the forces in the BUSH element (which will not show up as MPCFORCE output but ELFORCE output). Two methods for rigid elements are available, i.e. the linear method and the Lagrange method (see Section 6.3.23). The rigid elements are not real elements, they are internally represented by a set of MPC equations. By using these MPC equations, the dependent degrees-of-freedom (the m-set) are eliminated from the solution set. The rigid elements linear method has the following limitations; do not compute thermal load, do not have a differential stiffness matrix; therefore, the solutions are incorrect for the buckling analysis or other solution sequences where the differential stiffness matrix is required, use the small rotation theory in the geometrical nonlinear analysis so that the solutions are incorrect in this type of analysis, use the elimination method for solution, resulting in very dense stiffness matrices. These dense matrices cannot take advantages of the sparse matrix algorithm. The Lagrange method does not have the above limitations. With the Lagrange method, the rigid elements become “real” finite elements, similar to, for example, a QUAD4 element. Instead of using MPC equations, the element stiffness matrix is computed for each rigid element. Two solution methods are available, namely the Augmented Lagrange Multiplier Method (for this method, the solution is obtained with the independent degrees-of-freedom, the dependent degrees-of-freedom, and the Lagrange multipliers degrees-of-freedom left in the solution set. Thus, the sparse characteristic of the stiffness matrix is maintained and sparse matrix algorithms can be used) and the Lagrange Elimination Method (for this method, additional operations of eliminating both the dependent and Lagrange multiplier degrees-of-freedom from the solution set are performed after the global stiffness matrix is assembled. The solution is performed on the independent set (the n-set), creating dense matrices after elimination. Once again, these dense matrices cannot take advantage of the efficiency features of sparse methods). For most problems, the augmented Lagrange multiplier method is preferred. The tangent stiffness matrix using this method, however, is not positive definite, and can potentially pose numerical difficulties. The Lagrange elimination method is introduced as a backup for eigenvalue problems. The Lagrange elements are only available for linear static analysis (SOL 101), normal modes analysis (SOL 103), buckling analysis (SOL 105) and general nonlinear analysis (SOL 400) but not in SOL 106 and SOL 129. Note that the application of proper nonlinear rigid elements is one of the major benefits of SOL 400 to SOL 106 and SOL 129. The Lagrange elimination method is only recommended for eigenvalue analysis, it is not recommended in nonlinear static analysis (but Augmented Multiplier Method is fine for general nonlinear scheme SOL 400) for the following reasons. For nonlinear analysis, 1033 Structural Engineering Analysis and Design Second Edition the tangent stiffness matrix must be updated at each nonlinear iteration for the Lagrange elimination method. This implies that only the full Newton-Raphson method can be used, which conflicts with the general iteration solution scheme employed in MSC.Nastran. The Control Case command RIGID selects the type of rigid element. It has the following format: LINEAR will select the linear rigid elements, LAGR will select the Lagrange rigid element with the Lagrange multiplier method, and LGELIM will select the Lagrange element with the Lagrange elimination method. If RIGID command does not exist in the user Case Control file, the linear rigid element will be used for all solution sequences except SOL 400. For SOL 400, the default rigid element type is the Lagrange rigid element with the Lagrange multiplier method. The parameter LANGLE selects the method to represent the lager rotations, having the following values: LANGLE,1 -- use the Gimbal angle method. LANGLE,2 -- use the left rotation method. LANGLE,3 -- use the right rotation method. LANGLE=1 or 2 is the existing method. LANGLE=3 is the new method implemented for the Lagrange rigid elements and is the only method available for the Lagrange rigid elements. Therefore, if Lagrange rigid elements are present in a structural model, MSC.Nastran will automatically use LANGLE=3, and ignore user input on the LANGLE parameter. The parameters LMFACT and PENFN are the scale factor k and penalty function p for the Lagrange rigid element with the Lagrange multiplier method. The purpose of LMFACT and PENFN is to make the values of the stiffness matrix for the Lagrange rigid elements approximately equal in relative magnitude to those of the other elements in a structural model. Too small a value produces inaccurate results and too large a value poses numerical difficulties. Usually, the same value is assigned to both LMFACT and PENFN. Under special requirements, the user may assign different values to LMFACT and PENFN. For example, if and PENFN = 0.0, then the solution method becomes the pure Lagrange multiplier method instead of the augmented Lagrange multiplier method. However, the user must exercise caution when assigning different values to LMFACT and PENFN. The default value is 1.0e+5. for all solution sequences except SOL 400. For the nonlinear solution sequence SOL 400, MSC.Nastran will compute the appropriate default value in nonlinear iterations. 1034 Structural Engineering Analysis and Design Second Edition 6.11 Boundary Conditions 6.11.1 Single Point Constraints (SPCs) It is important to ensure that the SPCs restrain the rigid body motion of the model in all 6 degrees-of-freedom (translations in x,y,z directions, rotations about x,y,z axes). Failure to do so would cause singularity in the stiffness matrix in linear static analyses. Note that this applies even if the user is applying a balanced set of loads on the model (e.g. applying internal pressure in a closed pipe). In this case restraints in 6 degrees-of-freedom must be specified, although they would carry negligible loads. A special case of rigid body motion occurs when at least a part of the structure is weakly coupled to the structure, in which case a mechanism occurs causing the matrix to again be singular. Another application of SPCs is for applying symmetric or anti-symmetric boundary conditions by restraining the appropriate degrees-of-freedom on the plane of symmetry. However in dynamic analysis, a symmetric boundary will not incorporate all the modes. For instance, for a beam, symmetric boundary conditions will capture odd bending modes, whilst antisymmetric boundary conditions are required for the even modes. The SPC card can be used to specify constraints and enforced displacement on individual grids, whilst SPC1 cards are used to specify a similar constraint on many grids simultaneously. $ CASE CONTROL SPC = < SPC SID in Bulk Data Section > $ BULK DATA SPC SID G1 C1 D1 G2 C2 D2 G5 $ CASE CONTROL SPC = < SPC SID in Bulk Data Section > $ BULK DATA SPC1 SID C G1 G2 G3 G4 G7 G8 THRU G47 G78 …etc… Gi – grid ids Ci – component numbers Di – enforced displacement 1035 G6 Structural Engineering Analysis and Design Second Edition 6.12 Linear Optimization SOL 200 SOL 200 is applicable to SOL 101, SOL 103, SOL 105, SOL 108, SOL 111, SOL 112 and static aeroelastic. The analysis command in the Case Control Section specifies the type of analysis to be undertaken. $ EXECUTIVE CONTROL SECTION SOL 200 $ CASE CONTROL SECTION SUBCASE 1 ANALYSIS = STATIC SUBCASE 2 ANALYSIS = MODES 6.12.1 Objective Function and Constraints Response quantities that can be optimized for include weight, volume, natural frequencies, buckling load factors, displacements, velocities, accelerations, stresses, strains, forces, frequency or transient response displacements, velocity, acceleration, force and stress, trim, stability derivatives in a static Aeroelastic analysis, damping levels in flutter and whatever user-defined analytical equation supplied. The case control commands are as follows. $ CASE CONTROL SECTION DESOBJ(MAX DESGLB = < SUBCASE 1 DESSUB = < SUBCASE 2 DESSUB = < or MIN) = < ID of DRESP1 or DRESP2 > ID of global constraints defined by DCONSTR > ID of subcase dependent constraints defined by DCONSTR > ID of subcase dependent constraints defined by DCONSTR > The bulk data entries are described as follows. DRESP1 DRESP2 DCONSTR DCONADD DEQATN DTABLE defines responses computed directly by the analysis defines synthesized responses for design problems defines the response constraints defines constraint set combinations defines the user-defined equations defines a table of real constants that are used in equations in DEQATN Do not use 0.0 for lower or upper bounds on DCONSTR. 6.12.2 Design Variables and Constraints DVPREL1 and DVPREL2 defines the field of the property entries (model parameters) that needs to be optimized referring to DESVAR entries to define how the values are to be altered in order to be optimized. DVPREL1 defines linear relations the model parameters and the design variables whilst DVPREL2 defines nonlinear relations. DVPREL1 thus defines the basic relationship between the model parameters Pi and the various design variables as Pi = C0 + ∑ COEFFi x DVIDi i DESVAR DLINK defines the design variables defines the dependent design variables 1036 Structural Engineering Analysis and Design Second Edition Shape optimization is performed using the DVGRID bulk data entry (instead of DVPREL1 or DVPREL2) which references the design variables DESVAR. It defines the direction and magnitude of a grid variation for a given change in a design variable. 6.12.3 Optimization Control Parameters DSCREEN DOPTPRM specifies measures of constraint screening defines the optimization process control 6.13 Computational Memory and Processing Power Demand If the stiffness matrix is stored and processed as if it were a full matrix, the storage and processing time resources rapidly becomes prohibitive as the number of DOFs N increases. With regards to memory needs, a full square matrix stored without taking advantage of symmetry, requires storage for N2 entries. If each entry is an 8-byte (32bit) double precision floating-point number (note that single-precision floating-point numbers require 4-bytes or 16-bits), the required storage is 8N2 bytes. Thus, a matrix of order N = 104 would require 8×108 bytes or 800 MegaBytes (MB) for storage. For large N the linear static solution is dominated by the factorization of K. This operation requires approximately N3/6 floating point operation units. Fortunately a very high percentage of the entries of the master stiffness matrix K are zero. Such matrices are called sparse. There are clever programming techniques that take advantage of sparsity that fit certain patterns. These sparse matrix algorithms do not ignore non-zero terms that are far away from the diagonal. A common sparse matrix algorithm is the skyline storage method, which requires 8N3/2 bytes storage for two-dimensional problems. The factorization of a skymatrix requires approximately 0.5N2 floating-point operation units for two-dimensional problems. 1037 Structural Engineering Analysis and Design Second Edition 7 LS-DYNA Cards The input keyword file (.key) is order independent, case insensitive and multiple blocks of the same keyword can be defined if desired. A keyword deck is started with an asterisk (‘*’) in column one. A dollar sign (‘$’) in column one precedes a comment and causes the input line to be ignored. Each card is 80 character strings long; hence a 10field card will have 8-character string fields whilst an 8-field card will have 10-character string fields. 7.1 Keyword Format of Input Deck To flag input as a keyword file *KEYWORD To denote end of input file *END To specify title of analysis *TITLE To control CPU time for the termination of the analysis *CONTROL_CPU CPUTIME 7.2 7.2.1 Output Cards ASCII Output Files Default ASCII files are log file gives dynamic relaxation convergence factor information; added mass in mass scaling otf file gives smallest time steps and corresponding governing element modes; mass of model message file gives total CPU time of analysis after completion The most useful ASCII file is the glstat (cheap in storage), which gives the global data of the analysis. It includes the time step, the kinetic energy, the internal energy, the stonewall energy, the spring and damper energy, hourglass energy, system damping energy, sliding interface energy, external work and total energy. ASCII files such as BNDOUT and NCFORC are in general very, very, very expensive in storage. *DATABASE_GLSTAT DT = 0.01 DT = time interval between outputs The energy output control card is often required *CONTROL_ENERGY Hourglass Stonewall Interface Rayleigh Damping Energy Energy Energy Energy Note that KE + IE + Sliding Interface Energy + Hourglass Energy + Stonewall Energy + Damping Energy = Initial KE + External Work; If LHS > RHS, energy introduced artificially for example from numerical instability or sudden detection of artificial penetration through a contact surface. If RHS > LHS, energy absorbed artificially. To plot material energies *DATABASE_MATSUM 1038 Structural Engineering Analysis and Design Second Edition 7.2.2 BINARY Output Files Dynamic relaxation complete state low frequency graphical processing files (.rlf) (Cheap in storage) *DATABASE_BINARY_D3DRLF CYCL = 1 CYCL = output at every nth convergence check Transient complete state low frequency graphical processing files (.ptf) (Expensive in storage) *DATABASE_BINARY_D3PLOT LCDT BEAM NPLTC DT = 0.1 Time interval DT = Total Analysis Time / Number of States Desired Contact force low frequency graphical processing files (.ctf) (Expensive in storage) *DATABASE_BINARY_INTFOR LCDT DT = 0.1 Time interval = Total Analysis Time / Number of States Required Time history high frequency signal processing files (.thf) for nodes, beams, shells & solids (Very cheap in storage) *DATABASE_BINARY_D3THDT LCDT DT = 0.01 *DATABASE_HISTORY_ (HM: outputblock) Extra time history high frequency signal processing files (.xtf) (Very cheap in storage) *DATABASE_BINARY_XTFILE *DATABASE_EXTENT_BINARY Independent restart dump files (.dpf) written separately every specified number of cycles (V. expensive in storage) *DATABASE_BINARY_D3DUMP CYCL = 99999 Auxiliary dump files (.adf) written over every specified number of cycles *DATABASE_BINARY_RUNRSF CYCL = 99999 This is good to keep just in case we may need to increase the analysis time 1039 Structural Engineering Analysis and Design Second Edition 7.3 Node Cards *NODE (HM: nodes) TC RC NID X Y Z A node without any element will be attached a small mass and inertia. Generally, these mass-less nodes do not cause any stability problems except when they interact with the structure. 7.4 Stiffness Element Cards *SET_NODE (HM: entity sets) *SET_ELEMENT (HM: entity sets) *ELEMENT *NODE (HM: nodes) *PART (HM: comp collector) *SECTION (HM: prop collector) *MAT (HM: mat collector) *EOS (HM: prop collector) *HOURGLASS (HM: prop collector) Basic LS-DYNA element and property card structure Beam, shell and solid elements in LS-DYNA that use uniformly reduced numerical integration can develop zero energy deformation modes called hourglass modes, having a typically zig-zag appearance to a mesh. These modes are controlled numerically by either an artificial stiffness or viscosity, which resists the formation of these undesirable modes. A brick solid element requires 3 DOFs x 8 Nodes = 24 independent deformation modes. However, with a single integration point, the element provides 3 direct stresses + 3 shear stresses + 6 rigid body modes = 12 independent deformation modes. Hence, 12 deformation modes are not stiff and have to be suppressed. As the mesh gets distorted, the element accuracy is reduced and the timestep required for stability becomes smaller. The analysis may crash. To check the prominence of hourglassing, compute the hourglass energy and ensure that it is less than 10% of the total energy. Usually, it is the solid elements that produce the greatest hourglassing. To avoid hourglassing:(i) avoid subjecting single solid elements to bending exciting hourglass modes (ii) try to use solid elements with good aspect ratios (iii) avoid point loads, use pressure loads instead (iv) avoid single node or line contact (v) use the viscous or stiffness method to suppress hourglassing; use *CONTROL_HOURGLASS to define the global method of hourglass suppression and/or *HOURGLASS to defined hourglass suppression cards referred to by parts *PART 1040 Structural Engineering Analysis and Design Second Edition *CONTROL_HOURGLASS Hourglass IHQ Coefficient *HOURGLASS HGID IHQ QM IBQ Q2 Q1 QB QW IHQ=1 Standard LS-DYNA viscous hourglass suppression IHQ=3 Exact volume solid integration viscous suppression for high velocity models such as seismic analyses IHQ=5 Exact volume solid integration stiffness suppression for low velocity and small displacement models (vi) employ fully integrated elements (which are stiff in all the modes of deformation associated with its DOFs) especially where distortions are large, but this very significantly increases computational demand Single Integration Point Elements Fully Integration Elements Constant stress through element Stress varies across element Less accurate More accurate Cheap, as a single 8 integration points element is more expensive than 8 single integration point elements More expensive Susceptible to hourglassing as the element is not stiff in all deformation modes, hence not suitable for large distortions Not susceptible to hourglassing 1041 Structural Engineering Analysis and Design Second Edition 7.4.1 Spring Element Cards Discrete spring elements have 1 DOF at each of their 2 nodes. To define a spring element *ELEMENT_DISCRETE (HM: springs) Scale Factor PF Offset Prestress EID PID N1 N2 VID VID = 0 (local axes) spring acts along axis from N1 to N2 VID ≠ 0 (defined axes) and define an orientation vector *DEFINE_SD_ORIENTATION (HM: vectors) either fixed in space or based on the motion of two nodes *PART PID SECID MID EOSID HGID GRAV ADPOPT *SECTION_DISCRETE KD V0 CL FD CDL SECID DRO DRO = 0 translational spring in which case material cards define force-displacement curve DRO = 1 torsional spring in which case material cards define moment rotation curve TMID TDL To define elastic linear spring material *MAT_SPRING_ELASTIC Elastic MID Stiffness To define elastoplastic spring material with isotropic hardening *MAT_SPRING_ELASTOPLASTIC Elastic Tangent MID Yield Stiffness Stiffness To define elastic nonlinear spring material with an arbitrary load curve with strain effects if necessary *MAT_SPRING_NONLINEAR_ELASTIC LCR MID LCID To define a inelastic nonlinear spring material *MAT_SPRING_INELASTIC Unloading MID LCID CTF Stiffness To define nonlinear inelastic spring material with arbitrary load curves for loading and unloading with strain softening, kinematic hardening or isotropic hardening *MAT_SPRING_GENERAL_NONLINEAR Initial LCID LCID Initial Yield in MID BETA Yield in Loading Unloading Compression Tension 1042 Structural Engineering Analysis and Design Second Edition 7.4.2 Beam Element Cards Beam elements have 6 DOFs at each of its 2 nodes. The Hughes-Liu formulation has a single integration point along the length, hence models constant bending. The Belytschko-Schwer formulation on the other hand models linear variations in bending moment exactly. The latter beam hence models nodal forces and moments without any internal beam forces or moments exactly. Hence, to model a beam with a point load in the middle exactly, subdivide the beam into two finite beam elements with the common node at the position of the point load. A constant magnitude distributed load on a beam would have a parabolic variation of bending moment. This cannot be modeled exactly, but can be modeled approximately by a number of linear bending moment Belytschko-Schwer beam finite elements. The number of section integration points depends on the quadrature rule QR specified. To model pins at the ends of the beam, we could enable the pin flags within ELEMENT_BEAM. *ELEMENT_BEAM (HM: bar2) EID PID N1 N2 N3 RT1 RR1 RT2 RR2 LOCAL A plane through N1, N2 and N3 defines the principal plane r-s of the beam, RT1, RT2, RR1 and RR2 define end release conditions and LOCAL defines whether the coordinate system is global or local. *PART PID SECID MID EOSID HGID GRAV ADPOPT TMID *SECTION_BEAM SECID ELFORM Area Major Iss ELFORM QR/IRID =1 =2 =3 =4 =6 = 1.0 = 2.0 = 3.0 = 4.0 = 5.0 = IRID Shear Factor Minor Itt QR/IRID Cross Section Polar Irr Shear Area SCOOR Hughes-Liu (Single integration point along length, i.e. constant bending moment) Belytschko-Schwer resultant beam (Linear bending moment distribution) Truss Belytschko-Schwer full cross section integration Discrete beam/cable One integration point across section 2 x 2 Gauss quadrature rule across section 3 x 3 Gauss quadrature rule across section 3 x 3 Lobatto quadrature rule across section 4 x 4 Gauss quadrature rule across section User defined integration rule quadrature rule as specified in *INTEGRATION_BEAM To set miscellaneous output parameters *CONTROL_OUTPUT Update Beam Reference Node Materials to model beams without yield *MAT_ELASTIC *MAT_LINEAR_DISCRETE_BEAM Materials to model beams with lumped plasticity at the ends *MAT_SEISMIC_BEAM *MAT_NONLINEAR_DISCRETE_BEAM *MAT_FORCE_LIMITED 1043 Structural Engineering Analysis and Design Second Edition The beam is elastic until the bending moment at the ends reaches the plastic capacity MP when plastic hinges form. The post-full yield behavior is governed by the moment-rotation curves and axial load-strain curves. Since, the axial collapse load is usually affected by the bending moment in the beam, a different axial collapse load curve needs to be specified for different values of end moments. Material to model concrete beam yielding *MAT_CONCRETE_BEAM Material to model tall shear walls such as chimneys *MAT_SEISMIC_BEAM *MAT_CONCRETE_BEAM To define user-defined integration rules QR/IRID *INTEGRATION_BEAM 7.4.3 Shell (QUAD4, QUAD8, TRIA3, TRIA6) Element Cards Shell elements have 5 DOFs at each node (no in-plane rotational DOF). By default it has a single integration point in plane and 2 integration points through the thickness. A fully integrated shell element will have 4 in plane integration points. Shells can be used either as shells (with bending and in-plane stiffness) or just as membranes (only in-plane stiffness). Thick shell elements have 8 or 6 nodes with nodes on top and bottom of the surface like a brick element. They have 3 translational DOFs at each node (no rotational DOFs) again like a brick element. By default it has a single integration point in plane and 3 integration points through the thickness. To provide controls for computing shell response *CONTROL_SHELL Shell Warpage Sorting of Shell Thickness Angle Degenerate Normal Change Limit Quads Update Enabling Default Shell Formulation Theory Warping Stiffness Enabling Plane Stress Plasticity Projection Method For Warping ADAPTIVE TMID To define QUAD4s or TRIA3s, *ELEMENT_SHELL_ (HM: tria3, quad4) EID PID N1 N2 N3 N4 The THICKNESS option overwrites that specified in *SECTION_SHELL. *PART PID SECID MID EOSID HGID *SECTION_SHELL_ (HM: prop collector) Number of Through Printout Shear SECID ELFORM Thickness Option Factor Integration Points NLOC T1 T2 T3 T4 Shell elements in ascending form of accuracy and cost 1044 GRAV Integration Rule ID QR/IRID ICOMP SETYP Fully Integrated Elements One Point Quadrature Structural Engineering Analysis and Design Second Edition Shell Element Formulation ELFORM Accuracy Cost Belytschko-Tsay (BT) 2 Flat geometry hence no warpage stiffness 1 Belytschko-Tsay with warping stiffness (BTW) Belytschko-Leviathan (BL) Belytschko, Wong, Chiang (BWC) 1.07 1.25 10 1.28 Co-rotational Hughes-Liu (CHL) 1.49 Hughes-Liu (HL) 2.45 Fully Integrated Belytschko-Tsay (FBT) Co-rotational Fully Integrated HughesLiu (CFHL) Fully Integrated Hughes-Liu (FHL) 2.80 8.84 20.01 ELFORM element formulation theory 1: Hughes-Liu (Accurate, expensive, non-planar geometry thus warpage modeled) 2: Belytschko-Tsay (Default, less accurate, cheap) 4: C0 triangular shell 5: Belytschko-Tsay membrane 9: Fully integrated Belytschko-Tsay membrane 10: Belytschko, Wong, Chiang (Inexpensive warping stiffness for Belytschko-Tsay) 12: Plane stress 13: Plane strain 16: Fully integrated version of Belytschko, Wong, Chiang To define user-defined integration rules QR/IRID, use *INTEGRATION_SHELL and to define viscous or stiffness hourglass control for under-integrated elements, use *HOURGLASS. To model non-yielding elastic, linear, isotropic materials *MAT_ELASTIC The inelastic, nonlinear, isotropic material model capable of defining either isotropic or kinematic hardening with strain-rate effects (for impulsive blast or projectile crash analysis) with the Cowper-Symonds rules *MAT_PLASTIC_KINEMATIC *MAT_PIECEWISE_LINEAR_PLASTICITY *MAT_PLASTICITY_WITH_DAMAGE *MAT_STRAIN_RATE_DEPENDENT_PLASTICITY To model reinforced concrete slabs yielding *MAT_RC_SHEARWALL To model reinforced concrete squat shear walls *MAT_RC_SHEARWALL *MAT_SPRING_SQUAT_SHEARWALL To define an eight node thick shell element *ELEMENT_TSHELL *SECTION_TSHELL *INTEGRATION_SHELL *HOURGLASS 1045 Structural Engineering Analysis and Design Second Edition 7.4.4 Solid (Brick, Wedge, Tetrahedral) Element Cards Solid elements have 3 translational DOFs at each node (no rotational DOFs). By default it has a single integration point, hence no bending resistance. A fully integrated HEX8 solid will have 8 integration points. The basic solid finite element is the brick. The wedge and tetrahedral elements are degenerate brick elements, i.e. the wedge is a brick element with one of the faces collapsed into an edge, and the tetrahedral element is a wedge with the edge collapsed into a point. The more degenerate an element, the less well it is likely to perform. Tetrahedral elements should therefore always be avoided. *ELEMENT_SOLID_ (HM: tetra4, penta6, hex8) EID PID N1 N2 N3 N4 N5 N6 N7 N8 ADAPTIVE TMID *PART PID SECID MID EOSID HGID GRAV *SECTION_SOLID_ AET SECID ELFORM ELFORM element formulation theory 1: Constant stress solid element 2: Fully integrated S/R solid To model non-yielding elastic, linear, isotropic materials *MAT_ELASTIC To model linear orthotropic elastic materials *MAT_ORTHOTROPIC_ELASTIC *MAT_ORTHOTROPIC_THERMAL *MAT_TEMPERATURE_DEPENDENT_ORTHOTROPIC The inelastic, nonlinear, isotropic basic bilinear elastoplastic material model with only isotropic hardening *MAT_ISOTROPIC_ELASTIC_PLASTIC The inelastic, nonlinear, isotropic material model capable of defining either isotropic or kinematic hardening with strain-rate effects (for impulsive blast or projectile crash analysis) with the Cowper-Symonds rules *MAT_PLASTIC_KINEMATIC *MAT_PIECEWISE_LINEAR_PLASTICITY *MAT_PLASTICITY_WITH_DAMAGE *MAT_STRAIN_RATE_DEPENDENT_PLASTICITY The hardening rule depends of β which the user can select as β = 0 for kinematic hardening where the diameter of the yield surface remains unchanged but the center can move and β = 0 for isotropic hardening where the center of the yield surface remains fixed and the diameter increases. A β value between these give a combination of the kinematic and isotropic hardening rules. This value of β affects the yield stress when the loading is reversed, e.g. what is the yield stress for compressive loading following yield in tension. Be sure to convert to true stress and true strain. Beyond the Ultimate Tensile Strength, the experimental curve is hard to interpret because all the deformation is concentrated in the neck region; it is recommended that the input curve be made flatter beyond UTS than the experimental curve to allow for the uncertainties. The failure strain should generally be set based on a reduction in cross-sectional area when the tensile test specimen fails. The unloading curve (hence inelastic material model) has the same stiffness as the initial elastic stiffness. 1046 Structural Engineering Analysis and Design Second Edition Variants of the bilinear theme include *MAT_ELASTIC_PLASTIC_THERMAL which allows properties to vary with temperature *MAT_ORIENTED_CRACK which includes fracture at predefined tensile stress *MAT_POWER_LAW_PLASTICITY where hardening parameters may exist in terms of an ‘n’ value To model concrete with both volumetric crushing and strain softening in shear (to simulate cracking) *MAT_SOIL_CONCRETE To model plastics *MAT_VISCOELASTIC To model rubber *MAT_MOONEY_RIVLIN_RUBBER Mooney-Rivlin rubber constants for rubber with Shore Hardness of 60 (ihrd 60) are presented. Material Parameter Density Poisson’s Ratio Parameter A Parameter B Property (mm, tonnes, N, sec) 0.9e-09 tonnes/mm³ 0.49 0.474 N/mm² 0.118 N/mm² Property (m, kg, N, sec) 900 kg/m³ 0.49 0.474e+06 N/m² 0.118e+06 N/m² To model fabrics *MAT_FABRIC To model glass *MAT_ELASTIC_WITH_VISCOSITY *MAT_LAMINATED_GLASS To model isotropic, inelastic (hence exhibiting hysteretic damping) and non-linear stiffness degrading (with strain) soil elements under cyclic loading such as during earthquakes *MAT_HYSTERETIC_SOIL *DEFINE_CURVE This is simply a non-linear material models where the material stress-strain curve is dependent upon the strain. In a linear material model, G = E/[2(1+ν)]. But in a non-linear material model, G is dependent upon the level of strain. The material model itself is of course still isotropic, i.e. same property in all directions, but non-linear. The non-linear soil material model simulates directly the non-linear shear stress-shear strain behaviour of soil loaded by strong cyclic seismic shear waves to large shear strain amplitudes. The shear stress - shear strain curves defining the soil elements’ constitutive models are derived from the G/G0 degradation curves (see Section 5.1.2.2). Let us look at typical examples on a project. We shall investigate the Sakhalin Tank Loading Unit (TLU), an offshore gravity base structure near Sakhalin Island, Russia weighing 82.7MN with fundamental frequency of about 1.0Hz and associated modal mass of about 9.7MN. At the site of the TLU, the sandy soil overlying the bedrock is approximately 2 m in depth. On the seabed surface, a leveling course (bedding layer) of gravel of 0.5 m thick is to be placed. At 2.5 m below the top surface of the soil and further downwards, the measured shear wave velocity is approximately 700.0 m/sec., indicating that the material below this level is sufficiently stiff to be considered as bedrock. Values of the small strain shear modulus, G0, for the five layers of soil elements are listed and the figure shows the normalised (to G0) shear stress - shear strain curves of the gravel bedding layer and the sand. 1047 Structural Engineering Analysis and Design Second Edition Lower Bound G0 (MN/m2) Best Estimate Upper Bound 1800 80.8 82.9 85.2 1800 97.0 99.0 102.0 Sand 1800 93.1 98.2 105.3 -1.0 to -1.5 Sand 1800 89.2 96.0 105.4 -1.5 to -2.0 Sand 1800 86.0 94.0 105.5 Soil Layer Depth (m) 1 0.5 to 0 2 0 to –0.5 Gravel Bedding Layer Sand 3 -0.5 to -1.0 4 5 Soil Type Density (kg/m3) While the horizontal response of the site soil to vertically propagating seismic waves depends on the non-linear deviatoric (shear) behaviour of the soil, the vertical response is determined by the volumetric behaviour, quantified by the bulk modulus of the soil material, which has to be entered into the material model. This is related to the shear modulus by G= E 2(1 + ν) Damping in the form of hysteretic damping within the model is explicitly accounted for due to the inelastic nature of the material model. To define viscous or stiffness hourglass control for under-integrated elements, use *HOURGLASS. 1048 Structural Engineering Analysis and Design Second Edition 7.5 Mass and Inertia Element Cards Lumped mass elements have no DOF but add user specified masses to their single nodes. *ELEMENT_MASS (HM: masses) EID NID MASS VALUE To define a lumped inertia element assigned to a node *ELEMENT_INERTIA EID NID CSID IXX IXY IXZ IYY IYZ IZZ CSID = 0 (global axes) CSID = (defined axes) and declare a *DEFINE_COORDINATE_NODES (from three defined nodes), *DEFINE_COORDINATE_SYSTEM (from three points) or *DEFINE_COORDINATE_VECTOR (from two vectors) 1049 Structural Engineering Analysis and Design Second Edition 7.6 Damping Cards To define mass weighted nodal damping that applies globally to the nodes of deformable bodies and to the mass center of the rigid bodies *DAMPING_GLOBAL To define mass weighted damping by parts of deformable or rigid elements *DAMPING_PART_MASS Higher frequency motions are under-damped and lower frequency motions are over-damped. To define Rayleigh stiffness damping coefficient by parts *DAMPING_PART_STIFFNESS Higher frequency motions are over-damped and lower frequency motions are under-damped. Other damping cards are *DAMPING_FREQUENCY_RANGE *DAMPING_MODAL *MAT_SEISMIC_ISOLATOR To define a energy dissipating viscoelastic damper with damping proportional to the velocity *ELEMENT_DISCRETE (HM: springs) *SECTION_DISCRETE *PART *DEFINE_SD_ORIENTATION (HM: vectors) *MAT_DAMPER_VISCOUS *MAT_DAMPER_NONLINEAR_VISCOUS To define a tuned-mass dampers *ELEMENT_MASS *ELEMENT_DISCRETE (HM: springs) *SECTION_DISCRETE *PART *DEFINE_SD_ORIENTATION (HM: vectors) *MAT_DAMPER_VISCOUS *MAT_SPRING_ELASTIC To model hysteretic dampers *MAT_SPRING_ELASTOPLASTIC or *MAT_SEISMIC BEAM To model viscoelastic bearing isolation devices *ELEMENT_DISCRETE *MAT_SPRING_ELASTIC *MAT_SPRING_ELASTOPLASTIC To model friction pendulum isolation devices *ELEMENT_DISCRETE *MAT_SPRING_ELASTIC *MAT_SPRING_ELASTOPLASTIC 1050 Structural Engineering Analysis and Design Second Edition 7.7 Rigid Element Cards and Structural Internal Constraints Only one amongst the cards of restraints, rigid bodies, prescribed motions, nodal constraints, stonewall, tied interface and spotwelds should apply to any one DOF in the structure. 7.7.1 Rigid Body 7.7.1.1 Formulation of Rigid Body Joint To switch the explicit rigid body joint treatment to an implicit formulation, which uses Lagrange multipliers to impose prescribed kinematic boundary conditions and joint constraints *CONTROL_RIGID Lagrange Joint Multiplier Stiffness Flag Formulation 7.7.1.2 Rigid Body With Mass And Inertia Properties From A Set Of Nodes *CONSTRAINED_NODAL_RIGID_BODY_ (HM: rigids RgdBody) NSID CID To define a node set, use *SET_NODE. If the coordinate system ID, CSID ≠ 0, declare a *DEFINE_COORDINATE_NODES (from three defined nodes), *DEFINE_COORDINATE_SYSTEM (from three points) or *DEFINE_COORDINATE_VECTOR (from two vectors) to define a local coordinate system. Use INERTIA option to in define inertia properties instead of calculating them. 7.7.1.3 Rigid Body With Mass And Inertia Properties From An Element *ELEMENT_BEAM *ELEMENT_SHELL_ (HM: tria3, quad4) *ELEMENT_SOLID_ (HM: tetra4, penta6, hex8) *PART_ EOSID HGID GRAV PID SECID MID Use INERTIA option to in define inertia properties instead of calculating them. ADAPTIVE TMID *SECTION_BEAM *SECTION_SHELL *SECTION_SOLID *MAT_RIGID MID Mass Density Young’s Modulus Poisson’s Ratio N COUPLE M ALIAS Constraints Translational Rotational Direction Constraints Constraints CMO CMO = 1.0 (global coordinate system) CMO = 0.0 (no constraints) CMO = -1.0, and declare a *DEFINE_COORDINATE_NODES (from three defined nodes), *DEFINE_COORDINATE_SYSTEM (from three points) or *DEFINE_COORDINATE_VECTOR (from two vectors) to define a local coordinate system. 1051 Structural Engineering Analysis and Design Second Edition The Young’s Modulus and Poisson’s Ratio is required for contact surface calculations. Note that different rigid bodies should reference different parts, as each part will have one mass and inertia property and will act as one rigid body even if all the elements of the part is not contiguous. 7.7.1.4 Extra Nodes on Rigid Bodies Extra nodes are added onto a rigid body so that (i) the response at a particular location can be recorded, or (ii) a load can be applied at a particular location (iii) joints can be attached at these nodes to join rigid bodies together (iv) springs (stiffness) or lumped mass in a particular direction can be attached The coordinates of the extra nodes are updated based on the motion of the rigid body. *CONSTRAINED_EXTRA_NODES_ NID or PID NSID PID defines the rigid body and NID or NSID defines the extra nodes to be added to the rigid body. *SET_NODE_LIST DA1 NSID NID NID NID NID 7.7.1.5 DA2 NID NID DA3 NID NID DA4 NID … NID … NID … NID … Merging Rigid Bodies To merge rigid bodies *CONSTRAINED_RIGID_BODIES *PART for master rigid body part *PART for slave rigid body part To define a joint between two rigid bodies (as tied nodes cannot be used on rigid bodies), *CONSTRAINED_JOINT_<...OPTIONS...>_ (HM: joints) *CONSTRAINED_JOINT_STIFFNESS_ The spherical joint is used to model pinned connections, the revolute a hinge connection and the cylindrical a hinge with sliding along its axis. 7.7.2 Rigidwall To define a rigidwall *RIGIDWALL_GEOMETRIC *RIGIDWALL_PLANAR This is a simplification of a contact surface which models a plane through which nodes cannot pass. This is used to model hard targets such as rigid walls defined by a vector normal to the plane of the rigid wall pointing out of the wall towards the model. Only nodes on the outside of the model need to be chosen as slave nodes. 1052 Structural Engineering Analysis and Design Second Edition 7.7.3 7.7.3.1 Constraints Between DOFs Interpolation Constraint The motion of a single dependent node is interpolated from the motion of a set of independent nodes. This is useful for: (i) the load distribution of a translational load or moment, applied to the dependent node to the surrounding independent nodes (ii) the modelling of shell-brick or beam-brick interfaces *CONSTRAINED_INTERPOLATION Dependent Dependent ID NID DOF Independent NID Independent DOF X Weight Factor Y Weight Factor Z Weight Factor Independent NID Independent DOF X Weight Factor Y Weight Factor Z Weight Factor … … … … … XX Weight Factor XX Weight Factor … YY Weight Factor YY Weight Factor … ZZ Weight Factor ZZ Weight Factor … To tie a beam to a solid with no common nodes for instance, the dependent node is a beam end node with dependent DOF 123456, and the independent nodes are a few nodes on the solid with DOF 123. If the beam node is shared, then the dependent DOF will be 123. To distribute a load, To define nodal constraint sets for translational motion (no rotational coupling) in global coordinates *CONSTRAINED_NODE_SET (HM: rigids ConNode) *SET_NODE To define linear constraint equations between displacements / rotations in global coordinates *CONSTRAINED_LINEAR (HM: equation) To constrain particular DOFs in order to model pins (tied in translation), rigid planes (tied vertically) etc, we can use tied nodes *CONTRAINED_TIED_NODES_FAILURE 7.7.4 Global Restraints To define a global boundary constraint plane *CONSTRAINED_GLOBAL Translational Rotational Constraint Constraint Direction of Normal X Offset 1053 Y Offset Z Offset Structural Engineering Analysis and Design Second Edition 7.7.5 7.7.5.1 Welds and Rivets Generalized Spot Weld *CONSTRAINED_GENERALIZED_WELD_ *SET_NODE *DEFINE_COORDINATE_ (HM: systems) if nodes coincident The generalized spotweld option includes a ductile failure in addition to brittle failure of the simple spotweld and allows for more than 2 nodes in the spotweld and for the nodes to be coincident. 7.7.5.2 Generalized Fillet Weld *CONSTRAINED_GENERALIZED_WELD_FILLET 7.7.5.3 Generalized Butt Weld *CONSTRAINED_GENERALIZED_WELD_BUTT 7.7.5.4 Generalized Cross-Fillet Weld *CONSTRAINED_GENERALIZED_WELD_CROSS_FILLET 7.7.5.5 Generalized Combined Weld *CONSTRAINED_GENERALIZED_WELD_COMBINED 7.7.5.6 Mass-Less Spotweld *CONSTRAINED_SPOTWELD The spotweld is defined by 2 non-coincident nodes and a brittle failure load. 7.7.5.7 Mass-Less Rivet To define a mass less rivet *CONSTRAINED_RIVET 7.7.6 Concrete Rebars To model reinforcement bars in concrete *CONSTRAINED_LAGRANGE_IN_SOLID *PART or *SET_PART or *SET_SEGMENT for slave elements *PART or *SET_PART for master solid elements 1054 Structural Engineering Analysis and Design Second Edition 7.8 7.8.1 Boundary Conditions Cards Single Point Constraints SPCs To apply essential boundary conditions, constraints of degrees of freedom can be applied on *NODE cards, but this not recommended and is only available for backward compatibility. Instead, it is better to explicitly define single point constraints *BOUNDARY_SPC_ (HM: constraints BoundSPC) NID or CID DOFX DOFY DOFZ NSID NID NID NID NID NID NID NID NID NID NID … NID NID NID NID DOFRX DOFRY DOFRZ NID NID … NID NID … NID NID … Rigid bodies should not be subjected to SPCs. Instead constraints on rigid bodies are applied on *MAT_RIGID. *SET_NODE_LIST DA1 NSID NID NID NID NID DA2 NID NID DA3 NID NID DA4 NID … NID … NID … NID … If the coordinate system ID is not global (CID ≠ 0) then it is necessary to define a local coordinate system i.e. declare a *DEFINE_COORDINATE_NODES (from three defined nodes), *DEFINE_COORDINATE_SYSTEM (from three points) or *DEFINE_COORDINATE_VECTOR (from two vectors) (HM: systems). 7.8.2 Non-Reflecting Boundaries To define a non-reflecting boundary for infinite solid element modelling such as infinite soil * BOUNDARY_NON_REFLECTING Dilatation Shear Segment Waves Waves Set ID Activation Activation In seismic analyses, it is sufficient to activate the shear waves flag only. Segments are equivalent to triangular or quadrilateral element faces on the boundary defined by listing corner nodes clockwise or anticlockwise. *SET_SEGMENT DA1 ID NID NID NID NID NID NID DA2 NID NID NID DA3 NID NID NID DA4 NID NID … 1055 NID NID … NID NID … NID NID … Structural Engineering Analysis and Design Second Edition 7.8.3 Contact Cards To control defaults for computation with contact surfaces *CONTROL_CONTACT The surface definition for contact is made up of segments on the shell or solid element surfaces. 7.8.3.1 Rigidwall Contact If the node penetrates the rigidwall, the normal velocity and acceleration is set to zero. 7.8.3.2 Surface To Surface Contact This is the most general contact definition, which includes penetration, separation and friction algorithms. It works by the penalty force method in which the penetration of one surface to another is resisted by a force. Contact is only between the defined slave and master surfaces. Make the smaller surface the slave and the larger surface the master. *CONTACT_AUTOMATIC_SURFACE_TO_SURFACE_TITLE (HM: interface) *CONTACT_CONSTRAINT_SURFACE_TO_SURFACE_TITLE The AUTOMATIC method is a penalty method (see Section 6.3.23). The soft option flag can be set if penetration is observed. The CONSTRAINT method is a Lagrange method and should be used if the soft option in the usual AUTOMATIC method is still not good enough to prevent penetrations. 7.8.3.3 Single Surface Contact This is used when a surface folds onto itself or where there is no separation into master and slave surfaces. It provides a generalized contact capability, which does not require identification of slave and master surfaces, i.e. any node on surface can contact any element. Hence the search logic is more complicated and more expensive than the surface-to-surface definition. *CONTACT_AUTOMATIC_SINGLE_SURFACE_TITLE 7.8.3.4 Nodes to Surface Contact This is a one-way contact surface treatment, the slave side is the nodes and the master side is the surface. It is used to model situations such as beam impacting a plate where the beam is not a ‘surface’. But the logic is similar to that for sliding with separation. *CONTACT_AUTOMATIC_NODES_TO_SURFACE_TITLE *CONTACT_CONSTRAINT_NODES_TO_SURFACE_TITLE 7.8.3.5 Eroding Contacts This is used in situations where the elements on the contact surface fail and have to be deleted, hence modifying the contact surface. 7.8.3.6 Tied Interface *CONTACT_TIED_SURFACE_TO_SURFACE *CONTACT_TIED_NODES_TO_SURFACE *CONTACT_TIED_SHELL_EDGE_TO_SURFACE This is used to glue different meshes together, hence providing a simple efficient way of mesh refinement. However, this can produce internal reflection of stress waves (although so can conventional mesh refinement). 1056 Structural Engineering Analysis and Design Second Edition 7.9 Restart Capabilities *RESTART To allow parts that is defined as deformable to rigid at the start on an analysis *DEFORMABLE_TO_RIGID_ *RIGID_TO_DEFORMABLE Computation cost can be significantly reduced by switching deformable parts that are not expected to deform to rigid parts. The analysis can be stopped and restarted with the parts switched back to deformable just when they are expected to deform. *STRESS_INITIALIZATION 1057 Structural Engineering Analysis and Design Second Edition 8 STRUCTURAL ENGINEERING 8.1 8.1.1 Conceptual Structural Design Spans and Span to Depth Ratios 1058 Structural Engineering Analysis and Design Second Edition 8.1.2 Steel Single-Storey Buildings Lateral stability checks should be made in accordance to Section 3.1.6.7 to account for possible P-∆ effects. 8.1.2.1 Universal Beam – Universal Column (No Pinned or Two-Pinned) Portal Frame The types of universal beam – universal column portal frame are: I. No Pinned (Rigid Bases), Rigid Eaves, Rigid Apex (Statical Indeterminacy, αs = 3) II. Two Pinned (Pinned Bases), Rigid Eaves, Rigid Apex (Statical Indeterminacy, αs = 1) The basic beam − column portal frame can span up to 60m. The portal frames spacing are usually 5-8m with 6m and 7.5m the most common. The eaves height is 6-15m. The purlin spacing is usually 1.5-2m for cladding performance (can support local loads and drainage requirements), erectability and economically designed restraint requirements. There is a need for an inclination (usually about 6°) in the roof for drainage, but for small spans (10m) the beam can be horizontal with the inclination being created by precambering or in the cladding finishes. Flat roofs are notoriously difficult to weather proof since deflections of the cross beam induce ponding of rainwater on the roof. Portal frames of low inclination also create substantial horizontal thrusts at the base. Alternatively, the portal frame cross beam can be inclined. The portal frame can be haunched at the eaves and/or apex where the bending moments are greatest. Lateral stability system is an important consideration. There are two directions to consider, in the vertical plane of the portal frame and the vertical plane orthogonal to it. In the vertical plane of the portal frame, lateral stability can be provided by rigid bases (i.e. cantilever columns) and/or by moment resistance at the eaves and apex, the latter of which is usual. The pinned base is more common to the fixed base portal frame, although the former results in a slightly heavier frame although the increase in frame cost is offset by the reduced foundation size. The portal frame must provide moment resistance at the eaves for the pinned base case, since it becomes a mechanism to lateral loads in the plane of the portal frame otherwise. With rigid bases and moment resistance at the eaves and apex, the frame is a rigid portal frame whilst with pinned bases and moment resistance at the eaves and apex, the frame is a two-pinned portal frame. Moment resistance at the eaves can be provided by adding a haunch member where although all connections are pinned, the eaves connection is effectively triangulated and together acts as a moment resisting connection. Alternatively of course, the connection can be designed as a moment resisting connection. In the vertical plane orthogonal to that of the portal frame, lateral stability is best provided by pin-jointed wind girder bracing elements at the gable end. The horizontal wind girder (often located within the depth of the cross beams) has to be supplemented by a vertical wind girder in the same bay to transmit the forces into the 1059 Structural Engineering Analysis and Design Second Edition foundations much like the multi-storey building in horizontal plane bracing arrangement described in Section 8.1.3.3. Of course, instead of the bracing arrangement, both the horizontal and vertical wind girder can be a reinforced concrete slab (or wall) or a moment resisting connection. The horizontal wind girder can be of two types. Type (a) which is a Warren bracing uses struts (often tubes) capable of resisting tension and compression. Type (b) uses less material but more members. The diagonals are tension only (wire ropes) and the orthogonal compression strut is of the shortest possible length. Similar arrangements must be used for the vertical wind girder in the same bay to carry the forces to the foundations. The two bracings systems are shown below. Note the in roof plane tie members to transfer the loads to the in roof plane girder which in turn transfers load to the vertical stability elements. These tie members also act to restrain the compression members from buckling. 1060 Structural Engineering Analysis and Design Second Edition The portal frame can be optionally tied. The portal can also be tied at the eaves to reduce the spread and the size of the rafter, although the headroom becomes restricted. For tied portals, it is mandatory that a second order analysis is performed for the in-plane stability analysis, instead of a simple P-∆ analysis. This is because the high tensile force in the ties would cause it to elongate and thus would allow the eaves to spread under gravity. This in turn causes a downward deflection in the apex, hence reducing the lever arm between the rafter and the tie which increases the tension in the tie and compression in the rafter. The dominant load case governing strength of frame is usually snow load (unless eaves height is large in relation to span), which is generally 0.6kN/m2. However, with sloping roofs of multiple spans and parapets, the action of drifting snow need to be considered (especially on the purlins and cladding) according to BS 6399-3. Most popular purlin sections are cold-formed computer numerically controlled (CNC) Zed, modified Zed and Sigma. The disadvantage of the Zed is that the principal axis is inclined to the web hence out of plane displacement occur or out-of plane forces are generated. The modified Zed has a principal axis inclination which is much reduced whilst the Sigma has a shear centre almost coincident with the load application line. Portal frames analyzed using a plastic collapse analysis method (Section 3.3.6.1) as opposed to a linear elastic analysis method tends to be more economical in weight. If plastic design is employed, then the plastic load factor λP must be ensured to be greater than the P-∆ amplification which is a function of the elastic buckling load factor, λE as presented in Section 3.1.6.7. Also, if plastic design is utilized, then the sections must have sufficient rotation capacity, i.e. they must be classified as plastic, not even compact. For the SLS, excessive lateral deflections can be reduced by increasing rafter size, fixing bases and having a haunch as that is the location of high bending moments. 1061 Structural Engineering Analysis and Design Second Edition 8.1.2.2 Universal Beam – Universal Column (Three-Pinned) Portal Frame The types of universal beam – universal column three pinned portal frame are: I. Rigid Bases, Pinned Eaves, Pinned Apex (Statical Indeterminacy, αs = 0) II. Pinned Bases, Rigid Eaves, Pinned Apex (Statical Indeterminacy, αs = 0) Moment resistance at the eaves can be provided by adding a haunch member where although all connections are pinned, the eaves connection is effectively triangulated and together acts as a moment resisting connection. Alternatively of course, the connection can be designed as a moment resisting connection. The three-pinned portal is statically determinate. Hence an elastic method of analysis is performed with a plastic design methodology. A plastic collapse analysis cannot be performed as the onset of the first plastic hinge denotes a plastic collapse since the degree of statical inderminacy is zero. No further redundancy is present in the system to warrant a plastic collapse analysis. The horizontal thrust is (ωL2/8)/H where H is the height to the apex. The moment at the eaves is H.a where a is the height to the eaves. 1062 Structural Engineering Analysis and Design Second Edition 8.1.2.3 Truss – Stanchion Portal Frame The types of truss – stanchion portal frame are: I. Rigid Bases, Rigid Eaves (Finite Eaves Depth) (Statical Indeterminacy, αs = 3) II. Pinned Bases, Rigid Eaves (Finite Eaves Depth) (Statical Indeterminacy, αs = 1) III. Rigid Bases, Pinned Eaves (No Eaves Depth) (Statical Indeterminacy, αs = 1) IV. Pinned Bases, Pinned Eaves (No Eaves Depth), Diaphragm Roof To Braced Wall in the Plane of the Portal Frame (Statical Indeterminacy, αs = −1 Without Diaphragm and Braced Wall) The truss and stanchion system is essentially an extension to the beam and column system to increase spans. Lateral stability system is an important consideration. There are two directions to consider, in the vertical plane of the portal frame and the vertical plane orthogonal to it. In the vertical plane of the portal frame, lateral stability can be provided by rigid bases (i.e.cantilever columns) and/or by moment resistance at the eaves for trusses with a finite depth at the eaves, the latter of which is not usual. The portal frame can be pinned base or fixed base. The portal frame must provide moment resistance at the eaves for the pinned base case, since it becomes a mechanism to lateral loads in the plane of the portal frame otherwise. With rigid bases and moment resistance at the eaves, the frame is a rigid portal frame, with pinned bases and moment resistance at the eaves, the frame is a two-pinned portal frame, and with rigid bases and no moment resistance at the eaves, the frame is a two-pinned portal frame. Moment resistance at the eaves is provided by the finite depth of the truss. If this is not provided or to further enhance the capacity of connection if a finite depth is provided, a haunch member can be added. In the vertical plane orthogonal to that of the portal frame, lateral stability is best provided by pin-jointed wind girder bracing (say Warren bracing) elements at the gable end. The horizontal wind girder is in the plane of the bottom booms and rafter and the vertical wind girder is located in the same bay to carry the forces into the foundations, much like the multi-storey building in horizontal plane bracing arrangement described in Section 8.1.3.3. Of course, instead of the bracing arrangement, both the horizontal and vertical wind girder can be a reinforced concrete slab (or wall) or a moment resisting connection. The portal frame can be optionally tied. Compression member buckling restraint is an important consideration for truss and stanchion systems. Under gravity, top chord members are restraint by the purlins which support the roof cladding. In the case of load reversal. The bottom chord must be restrained. A method would be to use ties on the bottom chord running the entire building length. Another solution would be to use a compression strut from the chord member to the roof purlin. 1063 Structural Engineering Analysis and Design Second Edition The eccentricity, e at the connection between the centerlines of the braces to the chord that may result will have an effect on the induced bending moments at the joint and the members. This eccentricity moment (calculated simply by the sum of the horizontal components of the bracing member forces multiplied by the nodal eccentricity, e) should be added to the effects obtained from the computer analysis in the design of the chord, braces and also the joint. It is customary to proportion this secondary bending moment to the connecting members in relation to their stiffnesses. The effect of secondary moments especially in heavily loaded members can at times cause an increase in the section size. In such cases, consideration should be given to the use of gusset plates to ensure connections are coincident at the node points. In some instances, omission of alternate columns may be permitted. Vertical load from intermediate truss can then be transferred using long-span eave beams; and lateral loading from intermediate truss can be transferred by in plan bracing to points of vertical bracing or vertical cantilevers (i.e. rigid base columns). 8.1.2.3.1 Warren Truss Warren Truss; Warren trusses have equal length tension and compression web members. They have about half the number of bracing members and half the number of connections to Pratt trusses. Warren trusses are also more open. The force in the chord at midspan is (ωL2/8)/d whilst the force in the diagonal web member at the support is (ωL/2).(S/d) where S is the length of the web member. 8.1.2.3.2 Modified Warren Truss (i.e. Warren Truss with Vertical Brace Elements) The modified Warren truss (with vertical brace elements) is used when loading is intended within the chord members instead of just at the joints in order to reduce bending moments in chord. It also is used to reduce effective buckling lengths of the chords. It can span greater distances than the Warren truss but uses more material to the Pratt truss. 1064 Structural Engineering Analysis and Design Second Edition 8.1.2.3.3 Pratt Truss Under vertical load, the longer diagonals are in tension and the shorter vertical braces are in compression. The disadvantage is that the compression chord is more heavily loaded than the tension chord at midspan. A disadvantage of the pitched Pratt roof truss is that wind loads may cause a reversal of load thus putting the longer web member into compression. 8.1.2.3.4 Howe Truss The Howe truss is the converse to the Pratt roof truss. For lightly loaded roofs under wind load causing a reversal of vertical load upwards, the Howe can be advantages. Another advantage is the fact that the tension chord is more heavily loaded than the compression chord at midspan under normal vertical loading. 8.1.2.3.5 Fink Truss The Fink truss offers savings in steel weight for long span high pitched roofs as the members are subdivided. For a Fink truss of span L, height 0.2L and subject to force W at each of the 9 equally spaced nodes on the roof, the force in the top chord at the support is tensile 1.18W, the force in the bottom chord at the support is compressive 1.09W and the inclined web member at the apex is compressive 0.47W. 8.1.2.3.6 Mansard Truss The Mansard truss is a variation of the Fink truss which has the advantage of reducing the unusable roof space. The main disadvantage is that the forces in the chords are increased because the depth is decreased. There could also be more connections to fabricate. 8.1.2.3.7 Vierendeel Truss 8.1.2.3.8 Saw-tooth Truss 1065 Structural Engineering Analysis and Design Second Edition 1066 Structural Engineering Analysis and Design Second Edition 8.1.3 Steel and Reinforced Concrete Multi-Storey (Potentially Tall) Buildings 8.1.3.1 Building Geometry and Anatomy 1067 Structural Engineering Analysis and Design Second Edition 1068 Structural Engineering Analysis and Design Second Edition Flooring Structure Retail 1 New Change London 75mm Screed 425mm Ribbed Floor Services 480mm Def + Tol Ceiling Headroom 50mm 70mm 5000 – 5500mm Component Office 1 New Change London 150mm Raised Floor 830mm Composite Beam Integrated Within Web Openings of 475mm 50mm 70mm 2750mm 1069 Structural Engineering Analysis and Design Second Edition 8.1.3.2 Vertical Gravity and Lateral Stability Systems Lateral stability elements should also be continuous from the foundations to the top of the structure it stabilizes, otherwise a provisions must be made for the transfer of forces to other bays. Lateral stability must be provided for both the orthogonal vertical planes. P-∆ effects should be incorporated in accordance to Section 3.1.6.7. 8.1.3.2.1 Rigid Base Frames (Buildings Up To A Few Stories) Frames which have a rigid base with the beams pinned into the columns are not very stiff to lateral loads. Note that when beams are pinned into the columns, at least one base has got to be rigid, otherwise the frame is a mechanism. 1070 Structural Engineering Analysis and Design Second Edition 8.1.3.2.2 Braced Frames (Buildings Up To 20 Stories) Braced frames are cantilevered vertical trusses (a.k.a. shear trusses) resisting lateral loads primarily through the axial stiffness of the frame members. Axial shortening and elongation of the column members under lateral loading accounts for 80 – 90% of the overall system deformation. Braces are usually steel and made of double angles, channels, T, tubes or wide-flange shapes. Braced frames are either concentric or eccentric. Concentric brace frames have all members intersecting at a point and have high stiffness but low ductility. Concentric brace frames can be X, diagonal or Modified Warren, Pratt or Howe, K or V, diamond or Petit. The Xbracing exhibits high lateral stiffness to weight ratio, but however creates a short circuit in the column gravity load transfer path as they absorb a portion of the column load in proportion to their stiffness, hence creating additional forces in both the diagonal and horizontal members of the X-bracing system. X-Bracing K-Bracing Pratt or Howe Bracing Diagonal Bracing (Modified Warren) V-Bracing Diamond Bracing Note that these bracing arrangements can be employed for multiple storeys at a time if the effective length is not prohibitive. This is illustrated for a two storey X-bracing and a 2 and 4 storey diagonal (modified Warren) bracing. X-Bracing Diagonal Bracing (Modified Warren) Diagonal Bracing (Modified Warren) The X-bracing causes a short circuit in the gravity load path. Vertical loads will produce axial loads in the bracing members and also produce a horizontal reaction at the base. This is depicted below for a pinned base braced portal frame. The beam is also pinned so that the lateral stability system does not include a moment resisting frame, but solely bracings. The vertical load at the ends of the beam depicts the large axial force coming down the columns whilst the smaller vertical beam load represents the load on the individual beam. Note the axial force in the bracing element and the thrust force at the base. The thrust is not particularly a problem as it can be resisted by having a tie element at the base. 1071 Structural Engineering Analysis and Design Second Edition K-bracing does not present a short circuit to the column gravity load, but does resist the vertical load of a particular floor. Hence a smaller axial load in the bracing and base thrust is observed. 1072 Structural Engineering Analysis and Design Second Edition V-bracing does not present a short circuit to the column gravity load, but does resist the vertical load of a particular floor. The Pratt and diagonal bracings do not resist the vertical columns loads nor a particular storey loads, hence no base thrust is observed. 1073 Structural Engineering Analysis and Design Second Edition Eccentric brace frames utilize axis offsets to introduce flexure and shear into the frame, which lowers the stiffness-to-weight ratio but increases ductility, ideal for seismic regions. Eccentric Pratt Bracing Eccentric K-Bracing Eccentic V-Bracing These vertical braced frames (so-called vertical cantilevered trusses) are often located in the elevator and service core areas as they can be enclosed within permanent walls. Braced frames in orthogonal planes can be joined to form closed section cells, which together are effective in resisting torsional forces. The aspect ratio of the bracing system matters for the magnitude of the push pull effect. The bracing is really just a vertical cantilever truss and the force in the chords is dependent the magnitude of the applied horizontal force and the lever arm between the chords. Hence, the slenderness ratio of these core trusses is of importance. As the core truss becomes more slender (i.e. a higher core truss with a smaller footprint area) the overall overturning effect manifests itself in increased axial forces in the chord members, i.e. the columns of the core truss system. Whilst these core truss chord members can be designed to resist tension forces, net foundation uplift is generally undesirable. Hence a design objective would be to spread the chords are far apart as possible whilst diverting gravity load to these chords to prevent or reduce the net tensile force. 1074 Structural Engineering Analysis and Design Second Edition 1075 Structural Engineering Analysis and Design Second Edition 8.1.3.2.3 Moment Resisting Frames (Buildings Up To 20 – 30 Stories) Moment resisting frames consist of horizontal and vertical members rigidly connected together in a planar grid form which resists lateral loads primarily through the flexural stiffness of the members, hence not very efficient. Moment resisting frames have the advantage of flexibility in architectural planning. They can be placed in or around the core, on the exterior or throughout the interior of the building. The size of beam members in a moment resisting frame often controlled by stiffness rather than strength in order to develop an acceptable drift. The lateral drift is a function of both the beam and column stiffness. As beam spans are often greater than story heights, the beam second moment of area has to be greater than that of the column by the ratio of beam span to story height for an effective moment resisting frame. Hence moment frames, effectively sized for lateral sway control, increase in column and beam size and stiffness from top to bottom in proportion to the lateral shear. On the other hand, for gravity loads, the column sizes increase from top to bottom but the beam sizes remain the same. Thus, it would be efficient if gravity loads applied on the beams were diverted to the beams of the moment resisting frames as much as possible due to their increases size (for stiffness) and hence strength capacity. As a first pass to the design of multi-storey buildings, a load take down must be performed. This distributes the forces from the floors onto columns according to the tributary area, thus making the assumption that all column supports on the floor are pinned and that they have the same vertical stiffness. 1076 Structural Engineering Analysis and Design Second Edition 8.1.3.2.4 Braced and Moment Resisting Frames (Buildings Up To 40 – 50 Stories) The linear wind sway of the moment frame when combined with the cantilever parabolic sway of the truss produces enhanced lateral stiffness. The truss is restrained by the frame at the upper part of the building whereas at the lower part the truss restrains the frame. In general core trusses are combined with moment frames located in the perimeter. 1077 Structural Engineering Analysis and Design Second Edition 8.1.3.2.5 Core and Shear Walls (Buildings Up To 35 – 40 Stories) Central cores and shear walls have been the most common system for lateral stability. Shear wall systems used for tall office buildings groups shear walls around service cores, elevator shafts and stairwells to form a stiff box type structure. In contrast with office buildings, high rise residential buildings have less demand for elevators, lobbies and services and hence do not usually have large stiff concrete shear wall boxes. A more common system will incorporate a small box structure around a smaller number of elevators and stair wells and include discrete shear walls between apartments. In both cases, the shear walls are designed to cantilever from the foundation level. Multiple shear walls throughout a tall building may be coupled to provide additional frame action and hence increase the overall building stiffness. Coupling can be realized by relatively shallow header or link beams within the ceiling cavity at each level or by means of one or two storey high shear coupling walls. By adding a coupling shear wall at a single level, reverse curvature is induced in the core above the coupling shear wall, significantly reducing lateral drift by increasing the overall building stiffness. As the building mass increase is minimal, there will be significant increase in the building natural frequency. Shear walls with returns work better than those without. Many tall buildings undergo torsional loading due to the nonalignment of the building shear centre (due to the asymmetry of the location of the shear wall boxes) with the location of the horizontal load application. Boxed shear wall systems provide an efficient means of resisting such torsion. Torsion is resisted by both warping and uniform shear. Particular care must be taken during computer modelling of boxed shear walls to reflect penetrations for elevator and stair doors, which affect the stiffness considerably. Reinforced concrete walls must be at least 180mm thick. 1078 Structural Engineering Analysis and Design Second Edition 8.1.3.2.6 Core and Outriggers (Buildings Up To 75 Stories) Central core boxes can be coupled via stiff beams or trusses, at discrete levels, to external shear walls or columns to achieve a stiff building structure. These outriggers serve to reduce the overturning moment in the core that would otherwise act as a pure cantilever, and to transfer the reduced moment to columns outside the core by way of a tension-compression couple, which takes advantage of the increased moment arm between these columns. Hence the uplift due to the core is reduced or eliminated along with the prohibitively high overturning forces in the building’s foundation system. Uplift should be avoided at all costs as that would result in the requirement of complicated rock anchor foundations. Piles are not able to resist uplift. Unlike the outrigger system, the core system inherently simply cannot take advantage of the entire with of the building to resist the lateral forces. Modern high-rise buildings frequently incorporate central elevator core along with generous column-free floor space between the core and the exterior support columns. Whilst greatly efficient, it also disconnects the two major structural elements available to resist the critical overturning forces present in the high-rise building and reduces it to the sum of the independent resistance of the individual structural elements, i.e. the core and the perimeter columns. But the incorporation of the outriggers will couple these two structural elements and enhances the systems ability to resist overturning forces dramatically. The system utilizes the perimeter gravity load resisting columns to resist the lateral loads. The most significant drawback of the outrigger system is their potential interference with occupy able and rentable space. This can be minimized or eliminated by locating outriggers in mechanical and interstitial levels or locating them in the natural sloping lines of the building profile. 1079 Structural Engineering Analysis and Design Second Edition 8.1.3.2.7 Tubular Systems (Buildings Up To 110 Stories) Tubular systems include framed tubes, trussed tube and the bundled tube. The organization of the framed tube system is generally one of closely paced exterior columns and deep spandrel beams rigidly connected together, with the entire assemblage continuous along each façade and around the building corners. The system is a logical extension of the moment resisting frame, whereby the beam and column stiffnesses are increased dramatically by reducing the clear span dimension and increasing the member depths, something which is not done within the building. The exterior column spacing is usually of the order of 1.5m to 4.5m centres. Spandrel beam depths for normal office or residential occupancy applications are typically 600m to 1200m. A benefit of the closely spaced and deep exterior members is in the total or partial elimination of the need for intermediate vertical mullion elements for cladding support. The resulting closely spaced beam-column frame arrangement approximates a tube cantilevered from the ground with openings punched through the tube walls. The framed tube system suffers from the “shear lag effect” i.e. that the columns in the middle of a side of the building is less stressed axially that the columns at the edges. Wind The more the distribution of the perimeter columns is similar to that of a fully rigid box cantilevered at the base, the more efficient the system will be. For the case of the solid walled tube, the distribution of axial force would be expected to be uniform over the windward and leeward walls and linear over the sidewalls as shown in red above. As the tubular walls are punched, creating beam-column frames, linear shear frame deformations are introduced due to shear and flexure in the tubular members as well as rotations of the member joints. This reduces the effective stiffness of the system as a cantilever. The extent to which the actual axial load distribution in the tube columns departs from the ideal is termed the “shear lag effect”. The forces in the columns towards the middle of the flange frames lag behind those nearer the corner and are thus less than fully utilized. Limiting the shear lag is essential for optimal development of the tubular system. A reasonable objective is to strive toward at least 75% efficiency such that the cantilever parabolic component in the overall system deflection under wind load dominates. The framed tube is usually made of reinforced concrete due to its inherent monolithic nature. The framed tube in structural steel requires welding of the beam column joint to develop rigidity and continuity. Often the formation of fabricated tree elements, where all the welding is performed in the shop in a horizontal position, has made the steel frame tube system more practical and efficient. The trees are then erected by bolting the spandrel beams together at midspan near the point of inflexion. The column spacing in steel framed tubular buildings must be evaluated to balance the needs for higher cantilever efficiency through closer spacing with increased fabrication costs. The use of deeper built up sections versus rolled members is also a matter of cost-effectiveness. The trussed tube system represents a classic solution for a tube uniquely suited to the qualities and character of structural steel. The ideal tubular system is one which interconnects all exterior columns to form a rigid box, which can resist lateral shears by axial forces in its members rather than through flexure. This is achieved by introducing a minimum number of diagonals on each façade and making the diagonals intersect at the same point at the corner column. The system is tubular in that the fascia diagonals intersect not only to form a truss in the plane but also 1080 Structural Engineering Analysis and Design Second Edition interact with the trusses on the perpendicular faces to affect the tubular behaviour. This creates the X form between corner columns on each façade. The diagonals can also be smaller Xs (instead of full cross façade), thus transforming each façade into a diagonalized braced frame form. A significant advantage of the trussed tube system is that relatively broad column spacing can be used in contrast to framed tube systems. The result is large clear spaces for windows, a particular characteristic of steel buildings. The larger spaced perimeter columns are especially welcome at the base of the building where architectural planning typically demands open access to the building interior from the surrounding infrastructure with as little encumbrance as possible from the exterior framework. Another advantage is that the façade diagonalization serves to equalize the gravity loads in the exterior columns, and this can have a significant impact on member proportions and foundation design. The framed and trussed tubular systems can readily be adapted to a variety of nonrectilinear, closed-plan forms, including circular, hexagonal, triangular, and other polygonal shapes. The most efficient shape is the square, whereas the triangular tube has the least inherent efficiency. The high torsional stiffness characteristic of the exterior tubular system has advantages in structuring unsymmetrical shapes. The bundled tube (or modular tube) was invented to cater for non-prismatic tubular systems. In the purest form, tubular systems are generally applicable to prismatic vertical profiles. For varying profiles and buildings involving significant vertical façade offsets, the discontinuity of the tubular frame to fit the shape suffers from serious inefficiencies. The need for vertical planning modulation and the control of shear lag for very tall buildings led to the development of the bundled, or modular tube concept. The bundled tube is more efficient because it was shown that the higher the aspect ratio of the building (i.e. the greater the ratio of height to the tube plan size with the perimeter column spacing and size kept constant), the greater the percentage of parabolic cantilever deflection component in the total lateral deflection at the top of the building. That is to say, the shear lag component is less significant. This led to the notion that if the overall tubular shape is structured into small cells in plan by the inclusion of interior tubular lines, then the overall structure would have the cantilever efficiency associated with that of a single cell with high aspect ratio. The interior tubular web lines serve to reduce the effect of shear lag on the column in the middle of the windward and leeward flange frames. The bundled tube concept allows for wider column spacing in the tubular walls than would be possible with only the exterior framed tube form. It is this spacing which makes it possible to place interior frame lines without seriously compromising interior space planning. The ability to modulate vertically can create a powerful vocabulary for a variety of dynamic shapes. 1081 Structural Engineering Analysis and Design Second Edition 8.1.3.3 In-Plane Stability (Diaphragm Action) Imagine a floor plan. The stability elements resisting the horizontal forces are situated at a particular location as shown by the thickened line below in the two orthogonal directions. In horizontal plane bracing must be provided to resist lateral loads in the two orthogonal directions. To transfer the lateral load (which is applied everywhere there is a mass) to these vertical stiffness elements, some sort of in plane transfer element is required. Tie members to transfer Y load to in horizontal plane truss girder, which in turn transfers load to the vertical stability elements. Y X Reinforced concrete floors and composite floors provide diaphragm action and hence transfer these lateral forces to the vertical stability elements. The absence of a reinforced concrete floor results in the need for in horizontal plane bracing or as a last resort by in horizontal plane moment resisting connection. The in horizontal plane bracing can be any of the types presented in Section 8.1.4.3 for a simply supported arrangement and in Section 8.1.3.2.2 for a cantilever arrangement, both deflecting in the horizontal plane. Above, the stability in the X direction is provided by a simply-supported arrangement with a modified Warren type bracing. Note that each of the 3 bays must be braced, continuous to the vertical stability system. The stability in the Y direction is provided by a cantilever arrangement with a combination of Pratt bracing, eccentric Warren bracing and eccentric V bracing. Again each of the 4 bays must be braced, continuous to the vertical stability system. There is also the need for in horizontal plane tie members to transfer the loads to the in horizontal plane truss girder which in turn transfers load to the vertical stability elements. All columns must be tied in to the framework, i.e. no part of an independent part of the structure shall be locally unstable. In other words, the existence of movement joints require that each separate part of the structure be independently stable. Each column should be effectively held in position by means of horizontal ties in two directions, approximately at right angles, at each principal floor level supported by that column. Horizontal ties should similarly be provided at roof level, except where the steelwork only supports cladding that weighs not more than 0.7 kN/m2 and that carries only imposed roof loads and wind loads. At re-entrant corners the tie members nearest to the edge should be anchored into the steel framework. All horizontal ties, and all other horizontal members, should be capable of resisting a factored tensile load, which should not be considered as additive to other loads, of not less than 75 kN. The horizontal ties may be: • steel members, including those also used for other purposes; • steel bar reinforcement that is anchored to the steel frame and embedded in concrete; • steel mesh reinforcement in a composite slab with profiled steel sheeting designed to act compositely with steel beams, the profiled steel sheets being directly connected to the beams by the shear connectors. 1082 Structural Engineering Analysis and Design Second Edition Disproportionate collapse is accounted for as follows. (a) (b) (c) If effective ties are provided, no other action is needed. To provide effective ties, every frame must be effectively tied at roof and floors and columns must be restrained in two directions at these levels. Beam or slab reinforcement may act as ties, which must be capable of resisting a force of 75kN at floor level and 40kN at roof level. This avoids catastrophic failures like the 1968 Ronan Point collapse. If ties are not provided, then a check is to be made to see if load bearing members can be removed one at a time without causing more than a specified amount of damage. If it is not possible to limit the damage to a specified amount, then the member concerned must be designed as a “protected” or “key” member. It must be capable of withstanding 34 kN/m2 from any direction. 1083 Structural Engineering Analysis and Design Second Edition 1084 Structural Engineering Analysis and Design Second Edition 8.1.3.4 Torsional Stability System Vertical stability elements should preferably be positioned symmetrically on plan to avoid torsional effects especially for tall buildings. 1085 Structural Engineering Analysis and Design Second Edition 8.1.3.5 Movement Joints Movement joints are employed in the following cases:I. II. III. IV. V. when there is a significant change in the type of foundation when there is a significant change in predicted settlement when there is a significant change in plan configuration when there is a significant change in the height of the building to break up large structures to avoid large thermal movements When detailed calculations are not undertaken, joints to permit movement of 15mm to 25mm should be provided at approximately 50m centres both longitudinally and transversely. In the top storey, joints should normally be provided to give a 25mm spacing. 1086 Structural Engineering Analysis and Design Second Edition 8.1.3.6 8.1.3.6.1 Transfer Structures Transfer Beam 1087 Structural Engineering Analysis and Design Second Edition 8.1.3.6.2 Transfer Vierendeel Presented is a study of the design of a transfer vierendeel at concept design on One New Change, London. Original Proposal The proposed member sections at the vierendeel are presented. Closed cells of enhanced members are chosen so that there is a uniform bending and shear load path. All members are rigidly connected for moment transfer except the floor below the vierendeel as shown pinned below. Mid columns are placed in the bay helping to reduced the bending moments and shear forces. The width of each bay is 9m with mid-columns separating at mid-span, the height 3.85m the second floor and above. Section Standard Beam Standard Column Size Fabricated I 700 x 400 x 30 x 35 Universal Column 356 x 406 x 287 kg/m 368.2 287.3 Enhanced Beam Fabricated I 700 x 600 x 40 x 50 659.4 Enhanced Column Fabricated RHS 500 x 500 x 70 x 70 945.1 The member utilization to the ULS load case is presented. 1088 Structural Engineering Analysis and Design Second Edition The bending moment, shear force and axial effects are presented. 1089 Structural Engineering Analysis and Design Second Edition 1090 Structural Engineering Analysis and Design Second Edition 1091 Structural Engineering Analysis and Design Second Edition The summary of the critical members is as follows. Effects Critical Column(s) Critical Beam(s) Bending moment All elevation columns directly next to support within span; Adjacent columns on either side to a lesser extent; All elevation beams directly next to support within span; Shear force As with bending moment; As with bending moment; Axial force Bottom elevation max compressive column on support line; Higher columns to a lesser extent; Bottom elevation max compressive beam next to support within span; Top elevation max tensile beam to lesser extent; Deflections are a consideration for cladding. 1092 Structural Engineering Analysis and Design Second Edition The span to depth for SLS is 1/165 and for live load alone is 1/410. Tie forces will have to be resisted by some sort of lateral stability system either directly or through diaphragm action to the lateral stability system. 1093 Structural Engineering Analysis and Design Second Edition Parametric Study – Effect of Simply Supported Back Span On comparison with the original scheme, generally all the members have higher utilization especially the members in the back span, now simply supported. As for the cantilever members, they also experience greater effects. The loads in the columns increase. The tie forces stay generally the same. 1094 Structural Engineering Analysis and Design Second Edition The deflections at the end of the cantilever also stay generally the same. Conclusion, this option cannot be more economical. Parametric Study – Removing Mid-Columns in Back Span Mid-columns help considerably within span, but to a much lesser extent in the back span. 1095 Structural Engineering Analysis and Design Second Edition The utilization is similar with original scheme. Tie force reactions are also similar as is the deflections. Conclusion, mid-columns in the back span contribute little to the resistance. If at all, it may be sufficient to incorporate mid-columns in only the first bay in the back span. Parametric Study – Extending Back Span to Another Bay Moment connection required between columns and beams within span and to an extent in the back span. An investigation is undertaken to determine the extent of back span required. On comparison with the original scheme, generally all the members have similar utilization. The loads in the columns are also similar as are the tie forces and the deflections at the end of the cantilever. Conclusion, this option cannot be more economical. Parametric Study – Vertical Support At Middle of Cantilever If a vertical support is added, then no enhanced members are required as shown by the utilization sketch below. 1096 Structural Engineering Analysis and Design Second Edition The tie forces decrease considerably. Conclusion 1097 Structural Engineering Analysis and Design Second Edition Scheme kg/m2 on Elevation Original 253 Simply-Supported Back Span By inspection greater than original scheme Removing MidColumns In Back Span 237 Extending Back Span to Another Bay By inspection similar to original scheme Vertical Support At Middle of Cantilever 186 Note that the columns have not been optimised, i.e. smaller sections are possible higher up the building. However the comparison above should still approximately hold. 1098 Structural Engineering Analysis and Design Second Edition 8.1.3.7 Structural Floor Systems Structural floor systems could be of I. II. III. Reinforced concrete (Section 8.4.3) Composite steel and reinforced concrete (Section 8.6.3) Prestressed concrete (Section 8.4.4) 1099 Structural Engineering Analysis and Design Second Edition 8.1.4 Steel, Reinforced Concrete and Masonry Bridges Typical spans for the different bridge options are presented. 1100 Structural Engineering Analysis and Design Second Edition 8.1.4.1 Steel and Reinforced Concrete Prismatic (Box or Plate) Girder Bridge A box girder produces a extremely torsionally stiff structure. This form lends itself well to composite construction for the top flange, but the box girder bottom flange tends to be embarrassingly wide whilst the plate girder bottom flange tends to be embarrassingly thick. Flat girder bridges are commonly built by cantilever erection, in which case the bottom flange has to carry compression over its whole length. For wide bridges (dual carriageways; 2 x 3 lanes + shoulders commonly add up to 30m width), the choice may be between twin boxes or 6 or 8 simple plate girders. The torsional stiffness of the boxes will probably make it economic to make two single box bridges structurally entirely separate in this case. As the span increases, dead load becomes relatively more important especially for highway bridges, so lightweight concrete may be economic for the deck; or even a stiffened steel plate deck. The latter is typically 15mm and stiffened by pressed steel troughs (roughly 8mm) on a module of 300mm. 300mm 300mm Simply supported constant depth composite girders for highway loading typically have span to depth of 20, whilst for railway the ratio is 15. Variable depth are appropriate if spans exceed 30m. 1101 Structural Engineering Analysis and Design Second Edition 8.1.4.2 Steel and Reinforced Concrete Haunched (Box or Plate) Girder Bridge For continuous composite girders of variable depth for highways the ratio is 25 at pier and 40 at mid span whilst those for railway are 30 and 60 respectively. 1102 Structural Engineering Analysis and Design Second Edition 8.1.4.3 Steel Truss Bridge Trusses are common for railway bridges due to their high stiffness since trains are much heavier than highway traffic. Typical load of trains are 80 kN/m per track and locally 4 axles of 250kN at 2m centres. Instead of explicitly accounting for dynamic effects, simplified dynamic design load is (1+φ) x static live load where φ = (V/V*) / (1−V/V*) where V is the train speed and V* is the speed at which train travels to traverse the entire span in 0.5T where T is the natural period of the bridge. The ideal span to depth ratio for trusses is found to be between 10 to 15, with 15 the optimum. Common planar bridge trusses include I. Warren Truss; Warren trusses generally provide the most economical solution since their long compression bracing members can take advantage of the fact that RHS are very efficient in compression. They have about half the number of bracing members and half the number of connections to Pratt trusses. Warren trusses are also more open. II. Modified Warren Truss (i.e. Warren truss with vertical brace elements); The modified Warren truss (with vertical brace elements) is used when loading is intended within the chord members instead of just at the joints in order to reduce bending moments in chord. It also is used to reduce effective buckling lengths of the chords. It can span greater distances than the Warren truss but uses more material to the Pratt truss. III. Pratt Truss; Under vertical load, the longer diagonals are in tension and the shorter vertical braces are in compression. The disadvantage is that the compression chord is more heavily loaded than the tension chord at midspan. The Howe is the counterpart to the Pratt truss. Ideally, the diagonals should be designed to be in tension instead of compression. Hence they should be orientated to be more Pratt-like. Even for multiple spans, the diagonals can be iteratively flipped until all of them are in tension. IV. Howe Truss; The Howe truss is the converse to the Pratt truss. An advantage is the fact that the tension chord is more heavily loaded than the compression chord at midspan under normal vertical loading. The disadvantage is that, unlike the Pratt truss, the diagonals are in compression. V. Parker Truss; The Parker truss is a variable depth Pratt truss for structural efficiency. However, the fabrication cost is high due to variable depth and inclination of webs and top chord. VI. K or V Truss 1103 Structural Engineering Analysis and Design Second Edition VII. Diamond Truss VIII. Petit Truss; This is a subdivided Pratt or Howe truss. IX. Vierendeel Truss; This is a moment resisting connection (between the chord and verticals) truss. Lateral stability in the two vertical planes must be provided. The first vertical plane is the plane of the truss and naturally the web bracing of the truss or the moment connection (Vierendeel truss) shall provide the stability. For the second vertical plane, cross sectional stability must be provided to prevent lozenging instability of the truss. If the deck is the top chord, then concentric bracing can easily be provided in cross section. However, if the bottom chord is the deck, then open space is required and the lozenging stability of the tubes in cross section must be provided by either one (or multiples) of the following four options. First, a moment resisting connection in the cross sectional plane can be provided between the vertical web elements and the top deck cross beams through the chord. Second, a moment resisting connection in the cross sectional plane can be provided between the vertical web elements and the bottom deck cross beams through the chord. Third, eccentric portal bracing can be provided in the cross sectional plane where appropriate and acceptable from an architectural space planning point of view as shown in cross section view below. Fourth, lateral supports external to the tube can be provided at the level of the top chord deck at intermediate sections along the bridge. The lack of a complete set of cross-sectional stability at each node results in the need to provide in-plane stability (diaphragm action) in the two horizontal planes, i.e. in the plane of the bottom chord and the plane of the top chord. Diaphragm action needs to be provided by either a reinforced concrete deck, by horizontal plane bracing (concentric or eccentric) or inefficiently with an in horizontal plane moment resisting connection. These will allow the transmission of lateral forces (whether nominal, wind or seismic, they are all distributed according to the mass) in in-plane shear forces to the lateral supports. The in horizontal plane bracing arrangement is similar to that provided for multi-storey buildings as described in Section 8.1.3.3, only this time, there is only one direction in plan to brace, i.e. the direction orthogonal to the longitudinal axis of the truss (as the longitudinal direction is stable since on either side of the solitary bay the vertical plane web bracing of the truss provides stability). Now the in horizontal plane bracing can be any of the types presented in Section 8.1.4.3 for a simply supported arrangement and in Section 8.1.3.2.2 for a cantilever arrangement, both deflecting in the horizontal plane. Below, a combination of bracing arrangements, namely Pratt, V and Warren is shown (some bracing omitted, should actually be continuous). Of course, this bracing arrangement must be continuous to transfer the forces to the lateral stability system in the vertical plane. If this arrangement is provided for the top deck, the bracing must be continuous to the cross-sectional (lozenging) lateral stability system in the vertical plane. Plan View 1104 Structural Engineering Analysis and Design Second Edition The vertical plane cross-sectional bracing is to be placed at certain locations along the length of the truss, i.e. not necessarily at each and every node location, so long as in-plane stability (diaphragm action) bracing is provided to span in between. However, if the vertical plane cross-sectional bracing is provided at each and every node location, a scenario is possible with the moment connection system between the verticals and the bottom deck cross beams, then clearly there not the need for any in-plane stability (diaphragm action) bracing, as each cross-sectional cell is stable like a portal frame. However, the resulting U-frame must be checked for global buckling instability. The modelling of boundary conditions on FE models of trusses must be performed carefully. Since the boundary conditions are not placed at the neutral axis of the truss, a simply supported truss is simulated when only one translational restraint is placed longitudinal to the truss. If two longitudinal supports are placed, then a thrust reaction develops. But then again, if that simulates reality, then so be it. An buckling effective length factor K = 0.9 can be used for compression chord and K = 0.75 can be used for compression bracing member. Trusses are usually made up of hollow structural sections, i.e. rectangular hollow sections (RHS) or circular hollow sections (CHS) due to nature of loading within the truss elements being primarily axial. Tubular trusses are hence also lighter than their non-tubular counterparts. The smaller sizes of the members will also reduce protection costs as their surface area is less. CHS are pleasing to the eye of beholder and offer efficient distribution of steel about centroidal axes, but specialized profiling is required at the connections. On the contrary, RHS on the other hand offer easy connection detailing. RHS also offer superior deck or paneling fitting if they are to be laid directly on the top chord of the truss. RHS are also easier to handle and fabricate in the factory. Brace members must be smaller in dimension than the chord members in order to avoid complicated connecting pieces. Chord walls should generally be thick and bracing walls thin for an efficient joint. Connections are usually welded. When connecting the braces to the chords, overlap weld connections have superior static and fatigue (fatigue is nearly always a serious consideration in railway truss bridges) strength to gap weld connections. However, usually gap connections are required if centroid of the brace members are to meet exactly at the centroid of the chord members. Gap connections are also the preferred option for ease of fabrication, fitting and welding than overlap connections. The eccentricity, e at the connection between the centerlines of the braces to the chord that may result will have an effect on the induced bending moments at the joint and the members. This eccentricity moment (calculated simply by the sum of the bracing member force components parallel to the chord multiplied by the nodal eccentricity, e) should be added to the effects obtained from the computer analysis in the design of the compression chord, but may be ignored in the design of the tension chord and the braces. Alternatively, this eccentricity moment can be explicitly incorporated within the computer analysis by the use of short rigid elements modelling the eccentricity between the centerline of the chord and the centerlines of the braces. Another possibility of section choice is to use RHS chords sections and I diagonals. Bolted connections are then usual. Fatigue (fatigue is nearly always a serious consideration in railway truss bridges) can be minimized in the main truss action by making the gusset integral with the chord members (i.e. gusset butt welded in shop), provided with appropriate corner radii and the I-diagonals site bolted to gusset. 1105 Bridge Truss Roof and Floor Truss Structural Engineering Analysis and Design Second Edition Chord Verticals and Diagonals Remark Angle Angle Lightly loaded; Bolted directly; No gusset plate required; T T Angle Double Angles Lightly loaded; Bolted directly; No gusset plate required; H Channel More heavily loaded; Gusset plate bolted connection; RHS (SHS) RHS (SHS) Welded connection; RHS (SHS) CHS Welded connection; RHS H Gusset plate bolted connection; H H Channel Channel Gusset plate bolted connection; 1106 Structural Engineering Analysis and Design Second Edition 8.1.4.4 Steel Portal Bridge 1107 Structural Engineering Analysis and Design Second Edition 8.1.4.5 Steel, Reinforced Concrete or Masonry Arch Bridge The horizontal thrust at the base of a three pinned arch is (ωL2/8)/H where H is the height to apex. Plastic collapse analysis is described in Sections 3.3.4.2 and 3.3.6.1. 1108 Structural Engineering Analysis and Design Second Edition 8.1.4.6 Steel Cable Stayed Bridge 1109 Structural Engineering Analysis and Design Second Edition 8.1.4.7 Steel Suspension Bridge The mathematics of a catenary loaded vertically is presented. The following does not account for the change of curvature due to the stretch in the cables, a nonlinear static analysis is required for that. But the solution is accurate for well curved cables. Knowing W and S, either T or d must be chosen to solve for the other. A computer analysis of a catenary loaded vertically requires a (geometrically) nonlinear static analysis, a.k.a. form-finding. When there is no initial prestress in the cables, a (geometrically) nonlinear static analysis can be performed with the gravity loads applied on the cable elements (which have defined EA but no EI) until convergence to the equilibrium position is achieved. 1110 Structural Engineering Analysis and Design Second Edition A tension prestressed cable loaded vertically (eg. London Millennium Bridge) provides vertical stiffness to bending. To be straight the cable must have an initial prestress and theoretically no weight. In order to carry the weight, the cable needs to sag to a radius R. Knowing S, W, T0 and EA, T is solved for iteratively using then the dip, d is worked out by calculating R from as an intermediate step before it is calculated from the following expression. By changing estimate of T0, d will change. Straight cables can be used for load carrying, but either the prestress, T0 or the deflection, d will be high. A computer analysis of a tension prestressed cable loaded vertically requires a (geometrically) nonlinear static analysis, a.k.a. form-finding. When there is some initial prestress designed into the cables to reduce deflections, a (geometrically) nonlinear static analysis is performed with the gravity loads applied and some element prestress loads (simulated with say element temperature loads) applied on the cable elements (which have defined EA but no EI) until convergence to the equilibrium position is achieved. With the external load, the curvature of the formfound cable depends on the relative magnitude of the element prestress and the external load. The greater the prestress in the element, the flatter the form-found geometry. 1111 Structural Engineering Analysis and Design Second Edition 8.1.5 Steel Towers 1112 Structural Engineering Analysis and Design Second Edition 8.1.6 Steel Masts 1113 Structural Engineering Analysis and Design Second Edition 8.1.7 Steel Space Roofs 1114 Structural Engineering Analysis and Design Second Edition 8.1.8 Steel Cable Roofs Concepts of cable supported structures that may be relevant are presented in Section 8.1.4.6 and Section8.1.4.7. For two way cable net structures, approximate calculations can be performed using the single cable equations presented in Section 8.1.4.6 whilst also employing the following equations. where P is the load per surface area and t1 and t2 are tension per unit width where a1 and a2 are the cable spacings and T1 and T2 the cable tensions. A computer analysis of a steel cable roof requires a (geometrically) nonlinear static analysis, a.k.a. form-finding. When there is no initial prestress in the cables, a (geometrically) nonlinear static analysis can be performed with the gravity loads applied on the cable elements (which have defined EA but no EI) until convergence to the equilibrium position is achieved. Often however, there is some initial prestress designed into the cables to reduce deflections, in which case a (geometrically) nonlinear static analysis is performed with the gravity loads applied and some element prestress loads (simulated with say element temperature loads) applied on the cable elements (which have defined EA but no EI) until convergence to the equilibrium position is achieved. With the external pressure load, the curvature of the surface form-found depends on the relative magnitude of the element prestress and the external pressure load. The greater the prestress in the element, the flatter the form-found surface. 1115 Structural Engineering Analysis and Design Second Edition 8.1.9 Steel Grandstands 8.1.9.1 Cantilever Grandstand 8.1.9.2 Front Girder Grandstand 8.1.9.3 Cable Suspended Grandstand 1116 Structural Engineering Analysis and Design Second Edition 8.1.10 Reinforced Concrete Shell Roofs A form-finding computer analysis is often useful in the design of arbitrarily shaped shell roof structures to define a least surface area shape that meets certain boundary constraints. A (geometrically) nonlinear static analysis can be performed with a set of displacement restraints and/or supporting elements of definite stiffness properties defining the boundaries of the required geometry and applying an element prestress force (simulated with say element temperature loads) on the arbitrary shell structure (which need not have defined EA and certainly not EI properties). Since there is no external pressure load on the structure, the form-found shape of the structure will be the shape having least surface area. Since the external pressure is zero, the shape of the structure that is formfound is not affected by the magnitude of the element pre-stress, so it may be set to any reasonable value. 1117 Structural Engineering Analysis and Design Second Edition 8.1.11 Timber Single-Storey Buildings 8.1.11.1 Beam – Column (No Pinned or Two-Pinned) Portal Frame The types of universal beam – universal column portal frame are: I. No Pinned (Rigid Bases), Rigid Eaves, Rigid Apex (Statical Indeterminacy, αs = 3) II. Two Pinned (Pinned Bases), Rigid Eaves, Rigid Apex (Statical Indeterminacy, αs = 1) Moment resistance at the eaves can be provided by adding a haunch member where although all connections are pinned, the eaves connection is effectively triangulated and together acts as a moment resisting connection. Typical rafter and purlin sizes are presented. 1118 Structural Engineering Analysis and Design Second Edition 8.1.11.2 Beam – Column (Three-Pinned) Portal Frame The types of universal beam – universal column three pinned portal frame are: I. Rigid Bases, Pinned Eaves, Pinned Apex (Statical Indeterminacy, αs = 0) II. Pinned Bases, Rigid Eaves, Pinned Apex (Statical Indeterminacy, αs = 0) Moment resistance at the eaves can be provided by adding a haunch member where although all connections are pinned, the eaves connection is effectively triangulated and together acts as a moment resisting connection. A three pinned portal frame (pinned at apex and bases) used for a swimming pool is now presented. The rafters are 178mm wide x 500mm deep members whilst the compression and tension columns are 178mm wide x 225mm deep LVL members. The loads acting upon the structure are the dead load, superimposed dead load of 0.238kPa (0.23kPa on slope but 0.238kPa on plan) and services of 0.1kPa, wind loading of a certain amount and live loading snow of 0.6kPa. The purlins transfer the load onto the rafters as point loads. Compression Column Tension Column Pins The existence of both the compression and tension columns effectively creates a moment connection at the eaves. 1119 Structural Engineering Analysis and Design Second Edition 8.1.11.3 Truss – Stanchion Portal Frame The types of truss – stanchion portal frame are: I. Rigid Bases, Rigid Eaves (Finite Eaves Depth) (Statical Indeterminacy, αs = 3) II. Pinned Bases, Rigid Eaves (Finite Eaves Depth) (Statical Indeterminacy, αs = 1) III. Rigid Bases, Pinned Eaves (No Eaves Depth) (Statical Indeterminacy, αs = 1) IV. Pinned Bases, Pinned Eaves (No Eaves Depth), Diaphragm Roof To Braced Wall in the Plane of the Portal Frame (Statical Indeterminacy, αs = −1 Without Diaphragm and Braced Wall) Domestic Industrial Truss Span To 16m Truss Spacing 1.5m to 2.0m centres 5.0m to 6.0m centres Purlin Type Solid Solid or composite Purlin Spacing At node positions 0.8 to 1.8m centres Rafter Cladding Tiles (0.575kPa on slope) Corrugated sheeting Ceiling Plasterboard and insulation (0.25kPa) Economy usually results in truss spacing increases with truss span. Transportation is frequently a problem with large trusses, trusses deeper than 3m and longer than 20m requiring special attention. BS 5268-3 gives standard member sizes for the chords (rafters and ceiling ties) and for the internal web members for domestic trussed rafter roofs. Lateral stability system is an important consideration. There are two directions to consider, in the vertical plane of the portal frame and the vertical plane orthogonal to it. In the vertical plane of the portal frame, lateral stability can be provided by rigid bases (i.e.cantilever columns) and/or by moment resistance at the eaves for trusses with a finite depth at the eaves. The portal frame can be pinned base or fixed base. The portal frame must provide moment resistance at the eaves for the pinned base case, since it becomes a mechanism (4 pinned frame) to lateral loads in the plane of the portal frame otherwise. 1120 Structural Engineering Analysis and Design Second Edition With rigid bases and moment resistance at the eaves, the frame is a rigid portal frame, with pinned bases and moment resistance at the eaves, the frame is a two-pinned portal frame, and with rigid bases and no moment resistance at the eaves, the frame is a two-pinned portal frame. Moment resistance at the eaves is provided by the finite depth of the truss. If this is not provided or to further enhance the capacity of connection if a finite depth is provided, a haunch member can be added. In the vertical plane orthogonal to that of the portal frame, lateral stability is best provided by pin-jointed wind girder bracing elements at the gable end. The horizontal wind girder is in the plane of the rafter and the vertical wind girder is located in the same bay to carry the forces into the foundations. In rafter plane gable end bracing Braced end wall In the plane of the frame, stability can be provided by moment connection at the eaves. If this is not provided (as shown here as four pinned frames), the rafter plane of the roof must act as a diaphragm which transfers the forces to the braced end wall. Roof diaphragm Vertical plane gable end bracing In the plane orthogonal to frame, stability provided by (in rafter plane) gable end bracing which transfers the forces to the (vertical plane) gable end bracing. The purlins act as the tie elements. The in rafter plane roof diagonals is an efficient bracing system for lateral stability in both the in truss plane and orthogonal to truss plane directions. For bracing in both directions clearly a 45 degree angle is best. Smaller angles also cause construction problems. 1121 Structural Engineering Analysis and Design Second Edition The design of bracing for parallel beam or parallel truss systems is covered by EC5. A series of n parallel members which require lateral supports at intermediate nodes A,B, a bracing system should be provided, which, in addition to the effects of external horizontal load (e.g. wind), should be capable of resisting an internal stability load per unit length q, as follows 1122 Structural Engineering Analysis and Design Second Edition The modification factor kf,3 is approximately 30.0. The horizontal deflection of the bracing system due to force qd only should not exceed length/750. The horizontal deflection of the bracing system due to force qd and any other external load (e.g. wind), should not exceed length/500. An alternative to having roof diagonals is to design a roof diaphragm. The use of sarking on top of the rafters eliminates the need for bracing, provided the sarking is moisture resistant plywood (minimum thickness 9mm) or chipboard (minimum thickness 12mm) or 16mm timber boarding. Additional bracing elements that increase overall stability are I. Longitudinal bracing at apex and other node points (i.e. purlins) II. Web chevron bracing Also, lateral bracing at the mid point of compression members may be required, this however just to avoid local member buckling. 8.1.11.3.1 Collar Beam Roof The Collar beam is a three pinned frame roof which must be designed for a thrust at its base as it does not have a tie element. 8.1.11.3.2 Tied Three Pinned Rafter Roof 1123 Structural Engineering Analysis and Design Second Edition A tied three-pinned portal frame roof with the inclusion of an additional dimension results in the tied threepinned pyramid roof. The structure is an assembly/drama building. Purlins Tied (by edge beam) threepinned hip rafter The pyramid roof consists of two diagonal main hip rafters 150mm x 650mm LVL. The hip rafter is a tied threepinned frame system. They are restrained in LTB and minor axis flexural buckling at the locations of the purlins which are 75mm x 500mm LVL. They are not restrained to flexural buckling in the major axis. The ring beam acts as the tie in tension for the horizontal thrust of the three-pinned frame. The horizontal thrust is resolved in the perpendicular directions as tension into the ring beam. The self-contained tied three pinned frame system rests on 200mm masonry walls. The loads acting upon the structure are the dead load, superimposed dead load consisting of roof coverings (tiles, felt, battens, insulation) of 0.93kPa (0.8kPa on slope but 0.93kPa on plan) and services of 0.2kPa, wind loading of a certain amount and live loading snow of 0.6kPa. The purlins transfer the load onto the rafters as point loads. 8.1.11.3.3 Traditional Swiss, German, Compound Swiss, Scissor Trusses The Swiss, German, Compound Swiss and Scissor trusses are presented. 1124 Structural Engineering Analysis and Design Second Edition 8.1.11.3.4 Mono-Pitch Warren Truss Spans to 9m. Span to depth to 4. Purlins should be placed at node points to avoid secondary bending on the chord rafter. 8.1.11.3.5 Fink Truss Span to depth to 8. Coefficients which multiply the top chord point loads W or a unit load at the apex to get the member axial force are presented. 1125 Structural Engineering Analysis and Design Second Edition 1126 Structural Engineering Analysis and Design Second Edition 8.1.11.3.6 Variable Depth Warren Truss Spans to 12m (domestic) and 15m (industrial). Span to depth to 8. Purlins should be placed at node points to avoid secondary bending on the chord rafter. 8.1.11.3.7 Variable Depth Howe Truss and Pratt Truss Span to depth to 8. Coefficients which multiply the top and bottom chord point loads W and Wc or a unit load at the apex to get the member axial force on a variable depth Howe truss are presented. 1127 Structural Engineering Analysis and Design Second Edition 1128 Structural Engineering Analysis and Design Second Edition Coefficients which multiply the top and bottom chord point loads W and Wc or a unit load at the apex to get the member axial force on a variable depth Pratt truss are presented. 1129 Structural Engineering Analysis and Design Second Edition 8.1.11.3.8 Parallel Chord (Constant Depth) Warren Truss Span to depth to 10. Coefficients which multiply the top and bottom chord point loads W and Wc or a unit load middle of the bottom chord to get the member axial force on a Warren truss are presented. 1130 Structural Engineering Analysis and Design Second Edition 1131 Structural Engineering Analysis and Design Second Edition 8.1.11.3.9 Parallel Chord (Constant Depth) Howe Truss and Pratt Truss Presented is the Howe truss. The Pratt truss have got the diagonals flipped. The former have diagonals in compression under downward gravity whilst the latter have them in tension. The reverse is true for wind uplift. Spans to 30m (industrial). Span to depth to 10. With parallel chord trusses, unlike variable depth trusses, the loads in the web members are frequently very large which causes some difficulty in providing adequate connections. The coefficients are shown below for a typical span to depth just to compare the values on the web members. The Pratt truss can also be variable depth to form a Spandrel truss. 1132 Structural Engineering Analysis and Design Second Edition With a parallel chord Pratt truss, when they are joined to a timber or steel column with connections at both the top and bottom chords, this effectively gives rotational fixity in a building subject to sway, the system then effectively becoming a two-pinned base portal frame assuming that the bases are pinned. On the other hand, when it is required to minimize the height of the perimeter wall, the Howe truss is favoured, and to provide the lateral stability in the plane of the truss, rigid bases are required or a roof diaphragm to span walls or bracings in the plane of the frame. Pratt Truss Howe Truss To model the parallel roof truss with a finite depth of eaves all members, the following is undertaken. The columns are modeled with beam elements with no rotational releases, although it is pinned at the bases. All the web elements are rotationally released on either end. Also, the chord elements adjacent to the columns are also released rotationally. This models a truss with its individual members pinned onto a continuous column, but because of the finite depth, effectively moment resisting at the eaves. Apart from local element bending, no element is then subject to bending moments, except for the columns. 1133 Structural Engineering Analysis and Design Second Edition Coefficients which multiply the top and bottom chord point loads W and Wc or a unit load at the middle of the top chord to get the member axial force on a Howe truss are presented. 1134 Structural Engineering Analysis and Design Second Edition Coefficients which multiply the top and bottom chord point loads W and Wc or a unit load at the middle of the top chord to get the member axial force on a Pratt truss are presented. 1135 Structural Engineering Analysis and Design Second Edition 1136 Structural Engineering Analysis and Design Second Edition 8.1.11.3.10 Bowstring (Variable Depth Modified Warren) Truss Spans to 30m (industrial). Span to depth to 10. The bowstring truss can be very economical for large span industrial applications. It is the current alternative to the traditional nailed Belfast truss. With uniform loading and no large concentrated loads, the arched top chord profile supports almost all the applied loading. A parabolic profile is most efficient theoretically for uniform loading, but practical manufacturing considerations usually make it more convenient or necessary to adopt a circular profile. Purlins can be placed between node points deliberately to offset the moment caused by the product of the axial tangential loading and the eccentricity of the chord. 1137 Structural Engineering Analysis and Design Second Edition The Bowstring truss can also have a curved bottom chord to form a Crescent truss. 8.1.11.3.11 Mansard (Variable Depth Modified Warren) Truss Spans to 30m (industrial). Span to depth to 10. The bowstring truss has the disadvantage of requiring curved members, this adding to manufacturing and erection costs. The Mansard is then an option to overcome this problem with straight chord members. 1138 Structural Engineering Analysis and Design Second Edition 8.1.12 Timber Multi-Storey Buildings 8.1.12.1 Timber Floors Typical span to depth ratios for timber are presented. Typical joists for floor and flat roofs are presented. 1139 Structural Engineering Analysis and Design Second Edition 8.1.13 Masonry Single- and Multi-Storey Buildings 8.1.13.1 Lateral Stability Systems Masonry walls must be at least 150mm thick. 1140 Structural Engineering Analysis and Design Second Edition 8.2 8.2.1 Appreciation of Loading, ULS and SLS Load Cases Load Cases Approximate appreciation of loads is paramount to the structural engineer. Roughly, 1MN is 100 tonnes and 1 tonne is 10kN. A light car weighs about 1 tonne (10kN) whilst a very heavy person weighs about 0.1 tonnes (1kN). The Imperial College Queens Tower may weigh 9000 tonnes (90000kN), the offshore Sakhalin II PA-B gravity platform may weigh 130,000 tonnes (1300MN), whilst the Heathrow Terminal 5 Visual Control Tower may weigh just 800 tonnes (8000kN). The force being applied onto a 2.1m diameter, 20m long pile underneath the London St. Pancras underground extension may be 800 tonnes (8MN). Load cases are that must be considered are presented. Dead load (BS 6399-1) Superimposed dead load (BS 6399-1) Live load (BS 6399-1) Wind load (as described in Section 5.4) Snow load (BS 6399-3) Thermal load Gas and bomb explosions (as described in Section 4.9.2) Vehicle Impact (as described in Section 4.9.3) Notional Horizontal Load (BS 5950-1:2000) Disproportionate Collapse (as described in Section 8.1.3.3) Fire Protection Period Typical densities for the dead load values are presented. Normal Weight Concrete = 24.0 kN/m3 1141 Structural Engineering Analysis and Design Second Edition Light Weight Concrete = 19.0 kN/m3 Steel = 78.5 kN/m3 Water = 9.8 kN/m3 Typical superimposed dead load (SDL) are presented. Flooring (timber) = 0.25 kN/m2 Floor finish (75mm screed) = 1.8 kN/m2 Raised floor = 0.5 kN/m2 Ceiling boards = 0.4 kN/m2 Ceiling with acoustic panel = 0.5 kN/m2 False ceiling = 0.25 kN/m2 Services (nominal) = 0.25 kN/m2 Services (HVAC) = 0.4 kN/m2 Demountable lightweight partitions = 1.0 kN/m2 Blockwork partitions = 2.5 kN/m2 External curtain walling and glazing = 0.5 kN/m2 on elevation External cavity walls (lightweight block/brick) = 3.5 kN/m2 on elevation 1142 Structural Engineering Analysis and Design Second Edition Typical live loads based on BS 6399-1 are presented. Residential (domestic) = 1.5 kN/m2 Hotel bedrooms = 2.0 kN/m2 Hospital wards = 2.0 kN/m2 Public dining rooms, lounges, cafes, restaurants = 2.0 kN/m2 Car park = 2.5 kN/m2 Normal office = 2.5 kN/m2 + 1.0kN/m2 for demountable partitions Classroom = 3.0 kN/m2 Laboratories = 3.0 kN/m2 Stairs, corridors, landings, aisles, balconies = 4.0 kN/m2 Retail = 4.0 kN/m2 + 1.0kN/m2 for demountable partitions Assembly areas = 5.0 kN/m2 High-spec office = 4.0 to 5.0 kN/m2 + 1.0kN/m2 for demountable partitions Office file rooms = 5.0 kN/m2 Factories and workshops = 5.0 kN/m2 Dance halls, gymnasia = 5.0 kN/m2 Concert halls = 5.0 kN/m2 Libraries = 7.5 kN/m2 Escape routes = 7.5 kN/m2 Plant Room = 7.5 kN/m2 1143 Structural Engineering Analysis and Design Second Edition Live loadings based on EC1 Part 1:2002 is presented. 1144 Structural Engineering Analysis and Design Second Edition Typical snow load is 0.6 kN/m2. Another load case is the Notional Horizontal Forces (NHF) which must also be accounted for to allow for the effects of practical imperfections such as lack of verticality. Notional Horizontal Forces is 0.5% of the factored vertical (1.4DL+1.4SDL+1.6LL) load (BS5950) or 1.5% of the factored vertical (1.0DL+1.4SDL) load (BS8110). Fire protection period is presented. 1145 Structural Engineering Analysis and Design Second Edition 1146 Structural Engineering Analysis and Design Second Edition 8.2.2 Load Factors The load factors according to BS 5950-Part 1:2000 are presented. BS 5950-Part 1:2000 generally specifies ULS load factors of 1.6, 1.4 and 1.4 for live, dead and wind loads. 1147 Structural Engineering Analysis and Design Second Edition 8.2.3 Load Combinations Combinations of firstly dead and live, secondly dead and wind and thirdly dead, live and wind load must be considered. The British Standard ULS load combinations are Combination 1A: 1.4Dead + 1.4SDL + 1.6Live + 1.6Snow Combination 1B: 1.4Dead + 1.4SDL + 1.6Live + 1.6Snow ± 1.0NHF Combination 2A: 1.4Dead + 1.4SDL ± 1.4mWind (1.4mWind > % (1.4 or 1.0) Dead) Combination 2B: 1.0Dead + 1.0SDL ± 1.4mWind (1.4mWind > % (1.0 or 1.0) Dead) Combination 3: 1.2Dead + 1.2SDL + 1.2Live + 1.2Snow ± 1.2mWind (1.2mWind > % (1.2 or 1.0) Dead) The % of Dead that the wind is limited to is 1.0% (BS 5950) or 1.5% (BS8110). The factors applied to this Dead above again refer to BS5950 or BS8110. The P-∆ amplification factor m can be calculated using the simplified Amplified Sway Method as described in Section 3.1.6.7. The British Standard SLS load combination is Combination 1: 1.0Dead + 1.0SDL + 1.0Live + 1.0Snow + 1.0Wind The Eurocode ULS load combinations (with live load including the usual variable live load, wind, snow and temperature load) are Combination 1: 1.35Dead + 1.35SDL + γpPrestress + 1.5Livei +1.5ψ0Liveother i The Eurocode SLS load combinations (with live load including the usual variable live load, wind, snow and temperature load) are Combination 1: 1.0Dead + 1.0SDL + 1.0Prestress + 1.0Livei +1.0ψ0Liveother i Combination 2: 1.0Dead + 1.0SDL + 1.0Prestress + 1.0ψ1Livei +1.0ψ2Liveother i Combination 3: 1.0Dead + 1.0SDL + 1.0Prestress + 1.0ψ2Live 1148 Structural Engineering Analysis and Design Second Edition The French Standard ULS load combination is Combination 1A: Combination 1B: Combination 1C: Combination 2A: Combination 2B: Combination 3: Combination 4: 1.35(Dead + Temp) + 1.5Live 1.35(Dead + Temp) + 1.5Snow 1.35(Dead + Temp) + 1.5Wind 1.35(Dead + Temp) + 1.4(Live + Snow) 1.35(Dead + Temp) + 1.4(Live + Wind) 1.35(Dead + Temp) + 1.35(Live + Snow + Wind) 1.0(Dead + Temp) + 1.0(Live + Snow + Extreme Wind) The factored loads should be applied in the most unfavourable realistic combination for the part or effect under consideration. In each load combination, a γf factor of 1.0 should be applied to dead load (and live load too if relevant) that counteracts the effects produced by other loads as follows. I. II. Wind uplift Sliding, overturning and tension in gravity resisting members due to lateral wind and lateral NHF Non uniform load combinations that produce the most severe effects should also be considered. I. Factored live and dead loading on alternate bays, others 1.0 dead load For the envelope of these combination cases (which are really factored combinations of the individual load cases), contour plots can only present either the maximum positive or minimum negative value at a time. That being the case, the alternative to presenting two plots is to present the signed absolute value which automatically accounts for the maximum positive and minimum negative in one plot. 1149 Structural Engineering Analysis and Design Second Edition 8.3 Standard Construction Material Properties Typically, the engineering stress-strain curve is used where the applied load is divided by the original area. In actuality, a decrease in cross-sectional area occurs (necking), causing the true stress-strain curve to exhibit higher stresses. Hence the engineering stress-strain curve is conservative. The engineering strain is the average linear strain obtained from The engineering stress is as follows for yield and ultimate The true strain (up to onset of necking) is True stress (up to onset of necking) is True strain (beyond necking) is Beyond necking, true stress must be calculated from actual measurements of load and instantaneous cross-sectional area from 8.3.1 Steel, Aluminium and Concrete Property Tensile Strength (MPa) Compressive Strength (MPa) Steel Yield Strength, σy BS EN 10025 S275 – 275 BS EN 10025 S355 – 355 BS EN 10137 S460 – 460 Yield Strength, σy BS EN 10025 S275 – 275 BS EN 10025 S355 – 355 Aluminium Concrete Yield Strength, σy EN 485-2 AW2104-T4 – 240 EN 485-2 AW2104-T6 – 390 Negligible. Yield Strength, σy EN 485-2 AW2104-T4 – 240 EN 485-2 AW2104-T6 – 390 Ultimate Strength, σult 30 to 50 1150 Structural Engineering Analysis and Design Second Edition BS EN 10137 S460 – 460 Hardening Modulus (MPa) Hardening Parameter Ultimate Failure Strain BS EN 10025 S275 – 1140 BS EN 10025 S355 – 1230 BS EN 10025 S275 – 1.0 BS EN 10025 S355 – 1.0 BS EN 10025 S275 – 0.199 BS EN 10025 S355 – 0.199 NB. Yield strain 0.0020 EN 485-2 AW2104-T4 – 1630 EN 485-2 AW2104-T6 – 1224 EN 485-2 AW2104-T4 – 1.0 EN 485-2 AW2104-T6 – 1.0 EN 485-2 AW2104-T4 – 0.131 EN 485-2 AW2104-T6 – 0.068 0.0035 Stiffness (GPa) E: 205.0 G: 76.9 Steel is isotropic. E: 70.0 G: 26.1 Aluminium is isotropic. Short term: E = 28.0 G = 11.7 Long term: E = 14.0 G = 5.8 Concrete is isotropic. Poisson’s Ratio, ν 0.3 0.33 0.2 Density, ρ (kg/m3) 7850 2700 2400 1.2E-5 2.3E-5 1.0E-5 Susceptible. See Section 6.3.28.2.2. Not susceptible because of crystalline structure. Not susceptible. Susceptible. See Section 5.5. Susceptible. See Section 5.5. Not susceptible in compression. Material Cost ₤ / kg Coefficient of Thermal Expansion, α (Strain/°C) Impact Resistance (Brittle Failure Toughness) Fatigue Fire Corrosion Resistance Creep Coefficient of Thermal Conductivity at 20°C, λ (W/m°C) Heat Capacity, c (J/kg°C) 140 1000 Electrical Conductivity Chemical Resistance UV Resistance Sustainability Transparency to Radio Frequency 1151 Structural Engineering Analysis and Design Second Edition Electromagnetic Considerations Mild Steel with Typical Cowper-Symonds Strain-Rate Parameters Material Parameter Density Young’s Modulus Poisson’s Ratio Yield Stress Hardening Modulus Hardening Parameter Strain-rate Parameter C Strain-rate Parameter P Failure Strain Property (mm, tonnes, N, sec) 7.85e-09 tonnes/mm³ 2.1e+05 N/mm² 0.3 200 N/mm² 500 N/mm² 1.0 1300 strain/s 5.0 No failure strain used Property (m, kg, N, sec) 7850 kg/m³ 2.1e+11 N/m² 0.3 2.0e+08 N/m² 5.0e+08 N/m² 1.0 1300 strain/s 5.0 No failure strain used Steel Grade 275 Strain-Rate Curves 8.3.2 Stainless Steel Stainless Steel 1.4306 (Roughly Equivalent to AISI 304L) BS EN 10088-2 1152 Structural Engineering Analysis and Design Second Edition Material Parameter Density Young’s Modulus Poisson’s Ratio Yield Stress Hardening Modulus Hardening Parameter Failure Strain Property (mm, tonnes, N, sec) 8.0e-09 tonnes/mm³ 2.0e+05 N/mm² 0.3 220 N/mm² 1445 N/mm² 1.0 0.372 Property (m, kg, N, sec) 8000 kg/m³ 2.0e+11 N/m² 0.3 2.2e+08 N/m² 1.445e+09 N/m² 1.0 0.372 Stainless Steel 1.4404 (Roughly Equivalent to AISI 316L) BS EN 10088-2 Material Parameter Density Young’s Modulus Poisson’s Ratio Yield Stress Hardening Modulus Hardening Parameter Failure Strain Property (mm, tonnes, N, sec) 8.0e-09 tonnes/mm³ 2.0e+05 N/mm² 0.3 240 N/mm² 1501 N/mm² 1.0 0.336 Property (m, kg, N, sec) 8000 kg/m³ 2.0e+11 N/m² 0.3 2.4e+08 N/m² 1.501e+09 N/m² 1.0 0.336 Stainless Steel 316L True Stress-Strain Curve Density 7.65 x 10-9 tonnes/mm³ (7.65 tonnes/m³) Young’s Modulus 200 000 N/mm² Poisson’s Ratio 0.3 Yield Stress 260 N/mm² Effective Plastic Strain Effective Stress (MPa) (200 GPa) (260 MPa) 0 0.002 0.01 0.0472 0.2135 0.335 0.4261 0.6 260 311 347 445 741 898 983 983 Stainless Steel Bolt A2-70 The piecewise linear plasticity stress-strain material model for stainless steel material A2-70 parameters are as follows. Density 7.69 x 10-9 tonnes/mm³ (7.69 tonnes/m³) Young’s Modulus 200 000 N/mm² Poisson’s Ratio 0.3 Yield Stress 600 N/mm² (200 GPa) (600 MPa) Material A2-70 Effective Plastic Strain Effective Stress (MPa) 0 600 0.00 5 720 0.01 8 780 0.04 1 820 0.09 7 890 0.14 7 930 Strain-rate enhancement of the yield stress accounted for using the Cowper-Symonds model 1153 0.19 7 950 0.247 970 Structural Engineering Analysis and Design Second Edition 1  ε& P 1+   C where ε&is strain-rate. The C and P values used for the bolts are given below Material C P A2-70 300 1.7 The ‘static’ (corresponding to a very low strain-rate of about 1.0E-6) failure plastic strain is 0.61. The factors upon which this value is scaled for higher strain-rates are as follows. Strain-rate 0.0 1.00E-06 0.001 3.0 10.0 10000.0 Factor on Plastic Failure Strain 1.0 1.0 1.0 0.82 0.71 0.71 Plastic Failure Strain 0.61 0.61 0.61 0.50 0.43 0.43 1154 Structural Engineering Analysis and Design Second Edition The basic design strength, py may generally be taken as the 0.2% proof stress given above as those are minimum values. The exception is Duplex 2205 where a maximum of 450N/mm² should be used and this should be verified by mill certificates. For duplex 2205 with thickness 10 1155 Structural Engineering Analysis and Design Second Edition 8.3.3 Cast Iron Cast iron is a brittle material and hence employs a Mohr-Coulomb failure criteria. Typical values of density, Young’s modulus, E, and Poisson ratio are 7890kgm-3, 160.0GPa and 0.25 respectively and the stress-strain curve 1156 Structural Engineering Analysis and Design Second Edition is presented below 28. The tensile yield stress is 5.0MPa whereas the compressive yield stress is 200.0MPa. Note that the E value recommended in BD21/01 (average) and the Railtrack Line Code of Practice is 114GPa. Measured stress v.s. plastic strain 400 Stress [MPa] 200 0 -200 -400 -600 -800 -0.012 -0.010 -0.008 -0.006 -0.004 -0.002 0.000 0.002 0.004 0.006 Strain Note that “strain” for the material curves refers to effective plastic strain. A factor of safety of 5 on the ultimate strength is usually suggested for use in compressive resistance equations and hence buckling formulae. 8.3.4 Wrought Iron Typical stress-strain behaviour of wrought iron (which is more ductile than cast iron) is presented 29. 28 29 Steel Construction Institute. Appraisal of Existing Iron and Steel Structures. Publication 138, 1997. Steel Construction Institute. Appraisal of Existing Iron and Steel Structures. Publication 138, 1997. 1157 Structural Engineering Analysis and Design Second Edition 1158 Structural Engineering Analysis and Design Second Edition 8.4 Reinforced Concrete Design to BS 8110-Part 1:1997 (Buildings) and BS 5400-Part 4 (Bridges) 8.4.1 ULS Rectangular Beam Design – Bending, Shear and Torsion Effects 8.4.1.1 Bending Effects Characteristic Strength of Concrete fcu = 30 to 50 MPa Yield Strength of Longitudinal Steel, fy = 460 MPa Partial Safety Factor for Concrete, γmc = 1.5 Partial Safety Factor for Steel, γms = 1.15 Young’s Modulus for Steel, Es = 2.05E11 N/m2 Yield Steel Design Stress, (fy / γms) Ultimate Concrete Design Stress, 0.67fcu / γmc Design Steel Yield Strain εy = (fy / γms) / Es Design Ultimate Strain for Concrete (all grades), εcc Effective Depth of Section, d Total Depth of Section, h Width of Section, b The depth of plastic neutral axis, x needs to be limited for an under reinforced section. In an under-reinforced section the failure occurs with the gradual yielding of the tension steel and not by the sudden catastrophic compression failure of the concrete. Thus the steel εy must be reached before the concrete εcc is reached such that the steel yields in tension before the concrete yields in compression. Hence basically, the lower the x value the more under-reinforced the section is. Theoretical limit (by similar triangles) for the depth of the plastic neutral axis, x = d / (1+ εy/εcc) to ensure under-reinforced section (value not used in design). Limit (maximum) of depth of plastic neutral axis based on the code (conservative), x = (βb - 0.4)d (value used in design). The maximum moment capacity is obtained when the maximum neutral axis depth is used whilst still maintaining an under-reinforced section. If the moment capacity M1 at this stage is less than the design moment, then either increase section dimension or employ compression steel. Check if compression steel is required by computing moment capacity M1 = Fcc.z = (0.67fcu/γmc).(0.9b.x).(d-0.45x) with x = (βb - 0.4)d; If M1 > Md then design as singly reinforced, but if M1 < Md then design as doubly reinforced. Design as singly reinforced. Define K=Md/fcubd2. Required lever arm z in order to resist the ultimate design moment Md, z = d[0.5+SQRT(0.25-K.γmc/1.34)]. Lower limit of z from z = d - 0.45x enforcing under-reinforced limit x = (βb –0.4)d. Upper limit of z of 0.95d to avoid rupture of the tensile reinforcement at failure. Area of tension steel required to resist this moment Md, As = γms.Md/(fy.z). Check 100As / bh < 4.0. Check 100As / bh > 0.13 for high-yield steel (note 0.24 for mild steel). Analysis of singly reinforced section. Assuming that the tensile reinforcement steel has yielded at ULS (i.e. under-reinforced), the depth of neutral axis x obtained from equilibrium, Fcc = Fst, i.e. (0.67fcu/γmc).(0.9bx) = (fy/γms).(As provided). Ensure section is under reinforced, i.e. x < (βb - 0.4) and x < d / (1+ εy/εcc). Plastic moment capacity assuming tensile steel has yielded at ULS (under-reinforced), Mcapacity = Fcc.z = (0.67.fcu/γmc).(0.9bx).(d0.45x). Design as doubly reinforced. To increase the moment capacity of the section, either use a bigger section or provide compression reinforcement. Thus design for a doubly reinforced section only if the moment capacity if not sufficient to accommodate the design moment in a depth limited section. Let Md = M1 + M2. Moment capacity of singly reinforced section, M1 = Fcc.z = (0.67fcu/γmc).(0.9b.x).(d-0.45x) with x = (βb - 0.4)d. Area of steel to resist M1, As1 from M1 = Fst . z = (fy/γms).As1.(d-0.45x). Additional moment that needs to be resisted, M2 = Md - M1. Depth to compression reinforcement, d'. Ensure compression steel has yielded when concrete yields, i.e. ensure εcu (x-d')/x > εy. Provide additional steel at both top and bottom, As2 from M2 = (fy/γms).As2.(d-d'). Area of tensile reinforcement required, Ast = As1 + As2. Area of compression reinforcement required, Asc = As2. 1159 Structural Engineering Analysis and Design Second Edition Analysis of doubly reinforced section. Assuming that the tensile and compression reinforcement steel has yielded at ULS (i.e. under-reinforced), the depth of neutral axis x obtained from equilibrium, Fcc + Fsc = Fst, i.e. (0.67fcu/γmc).(0.9bx) + (fy/γms).(As2) = (fy/γms).(As1 + As2). Check if tensile steel has yielded at ULS (for underreinforced section) εst = εcc(d-x)/x > εy. Check if compression steel has yielded at ULS (for under-reinforced section) esc = εcc(x-d')/x > εy. Plastic moment capacity assuming tensile and compression reinforcement steel has yielded at ULS (under-reinforced), Mcapacity = Fcc.z + Fsc.(d-d') = (0.67.fcu/γmc).(0.9bx).(d-0.45x) + (fy/γms).(As2) (dd'). The assumption in beams is that all the longitudinal normal stress arises due to bending, hence ignoring contribution from the axial force. Ensure Compressive Axial Force < 0.1fcc bh. If Compressive Axial Force > 0.1fcc bh such as in columns, then generate M-N diagram. The M-N diagram depicts that with a little axial compression, the bending moment capacity is increased because failure in tension due to bending governs. But with even more axial compression, the bending resistance decreases as the failure in compression due to the axial force governs. P/(fcubh) Failure in compression (axial governs) Failure in tension (bending governs) M/(fcubh2) ULTIMATE LIMIT STATE DESIGN OF RECTANGULAR RC SECTION BS 8110-Part 1:1997 Concrete and Steel Material Stress-Strain Curve Comments Units Reference Basic User Data 50 MPa Yield Strength of Steel, fy 460 MPa Partial Safety Factor Concrete, γmc 1.5 Table 2.2 BS8110-1:1997 1.15 Table 2.2 BS8110-1:1997 Characteristic Strength of Concrete fcu Partial Safety Factor Steel, γms Table 3.1 BS8110-1:1997 Material Stress-Strain Curve Youngs Modulus For Steel, Es Yield Steel Design Stress, (fy / γms) Ultimate Concrete Design Stress, 0.67fcu / γmc 200000 MPa 400.0 MPa 22.3 MPa Figure 2.1 BS8110-1:1997 Design Steel Yield Strain εy = (fy / γms) / Es 0.0020 Figure 2.2 BS8110-1:1997 Design Ultimate Strain For Concrete (all grades), εcc 0.0035 Figure 2.1 BS8110-1:1997 Assumptions:(1) Plane Sections Remain Plane, i.e. not so deep beam (2) All tension carried by steel rebars as concrete cracks in tensile region Section Dimensions Effective Depth, d (Based on Span/d Ratio (12 Simply, 6 Cantilever, 15 Continuous)) 484 mm Total depth of section, h 600 mm 1500 mm 40 mm Width, b (Based on 1/3 < b/d < 2/3, say b = d/2) Nominal Cover, Cnom 1160 Clause 3.3 BS8110-1:1997 Structural Engineering Analysis and Design Second Edition Check for Under-Reinforced Section Based on Linear Strain Distribution Diagram The depth of plastic neutral axis, x needs to be limited for an under reinforced section. In a under-reinforced section the failure occurs with the gradual yielding of the tension steel and not by the sudden catastrophic compression failure of the concrete. Thus εy must be reached before εcc is reached such that the steel yields in tension before the concrete yields in compression. Hence basically, the lower the x value the more underreinforced the section is. Theoretical limit (by similar triangles) for the depth of the plastic neutral axis, x = d / (1+ εy/εcc) to ensure under-reinforced section (value not used in design) 308 Degree of moment redistribution for formation of plastic hinges, providing adequate rotation at the critical sections 0.00 Limit (maximum) of depth of plastic neutral axis based on the code (conservative), x = (βb - 0.4)d (value used in design) 290OK mm % Table 3.6 BS8110-1:1997 mm Clause 3.2.2 BS81101:1997 Design Ultimate Plastic Moment Capacity Based on Rectangular 0.9x Concrete Compression Stress Block 1070 Ultimate Design Moment To Be Resisted Md kNm (a) Check required design whether singly or doubly reinforced The maximum moment capacity is obtained when the maximum neutral axis depth is used whilst still maintaining an under-reinforced section. If the moment capacity M1 at this stage is less than the design moment, then either increase section dimension or employ compression steel. Check if compression steel is required by computing moment capacity M1 = Fcc.z = (0.67fcu/γmc).(0.9b.x).(d-0.45x) with x = (βb - 0.4)d; If M1 > Md then design as singly reinforced, but if M1 < Md then design as doubly reinforced. No Need Compression Steel (b) Design as a Singly Reinforced Section Define K = Md /fcu bd2 Clause 3.4.4.4 BS81101:1997 0.061 Required lever arm z in order to resist the ultimate design moment Md, z = d[0.5+SQRT(0.25-K.γmc/1.34)] 448 mm Lower limit of z from z = d - 0.45x enforcing under-reinforced limit x = (βb - 0.4)d 353OK mm Upper limit of z of 0.95d to avoid rupture of the tensile reinforcement at failure 460OK mm Area of tension steel required to resist this moment Md, As = γms.Md/(fy.z) 5966 32OK Diameter of Rebars mm2 mm 9 Number of Rebars Required Area Provided 7238OK mm2 Check 100As / bh < 4.0 0.80OK % Check 100As / bh > 0.13 for high-yield steel (note 0.24 for mild steel) 0.80OK % 7238 mm2 96 mm (c) Analysis of the Singly Reinforced Section Provided Area of steel provided as above Assuming that the tensile reinforcement steel has yielded at ULS (i.e. underreinforced), the depth of neutral axis x obtained from equilibrium, Fcc = Fst, i.e. (0.67fcu/γmc).(0.9bx) = (fy/γms).(As provided) Ensure section is under reinforced, i.e. x < (βb - 0.4) and x < d / (1+ εy/εcc) Plastic Moment Capacity assuming tensile steel has yielded at ULS (underreinforced), Mcapacity = Fcc . z = (0.67.fcu / γmc ).(0.9bx).(d-0.45x) 1161 OKCheck 1276 OK kNm Clause 3.4.4.4 BS81101:1997 Clause 3.2.2 BS81101:1997 Clause 3.4.4.4 BS81101:1997 Clause 3.4.4.4 BS81101:1997 Structural Engineering Analysis and Design Second Edition Moment redistribution factor available whilst maintaining section as under reinforced, βb >= 0.4 + x/d ensuring βb >= 0.7 0.7 (d) Analysis of Singly Reinforced Flanged Section Width of web, bw Effective width, beff = b as above = bw + 0.2Lz (internal beam) or bw + 0.1Lz (end beam) Thickness of flange, t Area of steel provided as above (d)(i) Assume stress block within flange The moment capacity is the same as that of above for the perfectly rectangular section Check stress block within flange, i.e. 0.9x < t 300 mm 1500 mm 150 mm 7238 mm2 OK (d)(ii) Assume stress block within web Assuming that the tensile reinforcement steel has yielded at ULS, the depth of neutral axis x obtained from equilibrium, Fcflange + Fcweb = Fst, i.e. (0.67fcu/γmc).beff.t + (0.67fcu/γmc).(0.9x-t)bw = (fy/γms).As Ensure section is under reinforced, i.e. x < (βb - 0.4) and x < d / (1+ εy/εcc) Plastic Moment Capacity assuming tensile steel has yielded at ULS (underreinforced), Mcapacity = Fcflange.(d-0.5t) + Fweb.(d-0.5(0.9x+t)) = (0.67.fcu / γmc).(beff.t).(d-0.5t) + (0.67.fcu / γmc)(0.9x-t)bw.(d-0.5(0.9x+t)) Check stress block within web, i.e. 0.9x > t -186.5 mm OK 1005 kNm Warning (e) Design as a Doubly Reinforced Section To increase the moment capacity of the section either use a bigger section or provide compression reinforcement. Thus design for a doubly reinforced section only if the moment capacity if not sufficient to accommodate the design moment in a depth limited section. Let Mcapacity = M1 + M2 Moment capacity of singly reinforced section, M1 = Fcc.z = (0.67fcu/γmc).(0.9b.x).(d-0.45x) with x = (βb - 0.4)d 3094 kNm Area of steel to resist M1, As1 from M1 = Fst . z = (fy/γms).As1.(d-0.45x) 21889 mm2 Additional moment that needs to be resisted, M2 = Md - M1 -2024 kNm Depth to compression reinforcement, d' Ensure compression steel has yielded when concrete yields, i.e. ensure εcu (x-d')/x > εy Provide additional steel at both top and bottom, As2 from M2 = (fy/γms).As2.(d-d') Area of tensile reinforcement required, Ast = As1 + As2 50 OKCheck -11656 mm2 10233 mm2 32OK Diameter of Rebars mm mm 3 Number of Rebars Required Area Provided 2413Warning Area of compression reinforcement required, Asc = As2 -11656 20OK Diameter of Rebars 2 mm 2 mm mm 2 Number of Rebars Required 628OK mm2 Area of steel Ast provided as above 628 mm2 Area of steel Asc provided as above 2413 mm2 24 mm Area Provided (f) Analysis of the Doubly Reinforced Section Provided Assuming that the tensile and compression reinforcement steel has yielded at ULS (i.e. under-reinforced), the depth of neutral axis x obtained from equilibrium, Fcc + 1162 Structural Engineering Analysis and Design Second Edition Fsc = Fst, i.e. (0.67fcu/γmc).(0.9bx) + (fy/γms).(As2) = (fy/γms).(As1 + As2) Check if tensile steel has yielded at ULS (for under-reinforced section) εst = εcc(dx)/x > εy OKCheck Check if compression steel has yielded at ULS (for under-reinforced section) εsc = εcc(x-d')/x > εy WarningCheck Plastic Moment Capacity assuming tensile and compression reinforcement steel has yielded at ULS (under-reinforced), Mcapacity = Fcc . z + Fsc . (d-d') = (0.67.fcu / γmc ).(0.9bx).(d-0.45x) + (fy/γms).(As2) (d-d') 447 kNm (g) Analysis of the Doubly Reinforced Flanged Section (h) Check if there is significant compressive axial force within section The assumption in beams is that all the longitudinal normal stress arises due to bending, hence ignoring contribution from the axial force. 3200Entered Compressive Axial Force Ensure Compressive Axial Force < 0.1fcc bh ~ 0.1fcc b (d + Cnom) kN OKCheck Design For Combined Bending and Tensile or Compressive Axial Force This requires the generation of the M-N diagram 1163 Structural Engineering Analysis and Design Second Edition 8.4.1.2 Shear and Torsion Effects Characteristic Strength of Concrete fcu = 30 to 50 MPa Partial Safety Factor for Concrete, γmc = 1.5 Partial Safety Factor for Steel, γms = 1.15 Yield Strength of Link Steel, fyv = 460 MPa Yield Strength of Longitudinal Steel, fy = 460 MPa Effective Depth of Section, d Width of Section, b Area of Tensile Steel Reinforcement Provided, As Design shear force, V at d (BS 8110-Part 1:1997) or 2d (BS 5400-Part 4) from support. Design shear stress, vs = V / bd. Design torsional stress for rectangular sections, vt = 2T / ((hmin2)(hmax-hmin/3)). Torsional stress for thin hollow section, vt = T / (2Aht) where wall thickness of thin hollow section, ht and Area enclosed by center-line of thin hollow section, A. Design torsional stress for T-, L- or I-shaped divided into rectangular components and use T(hmin3.hmax)/ S(hmin3.hmax). Ultimate shear stress capacity for shear and torsion. Check design shear and torsion stresses vs + vt < vu, lesser of 0.8(fcu)0.5 or 5MPa whichever smaller (BS 8110-Part 1:1997). Check design shear and torsion stresses vs + vt < vu, lesser of 0.75(fcu)0.5 or 4.75MPa whichever smaller (BS 5400-Part 4). Shear capacity of concrete. Shear capacity of concrete, vc = (0.79/1.25)(100ρwfcu/25)1/3(400/d)1/4; 100ρw < 3; fcu < 40; (400/d)1/4 > 1.0 where tensile longitudinal steel ρw = As/bd (BS 8110-Part 1:1997). Nominal concrete shear capacity, Vnominal = bd(vc) (BS 8110-Part 1:1997). Shear capacity of concrete, ξsvc = (0.27/1.25)(100ρwfcu)1/3(500/d)1/4; 100ρw < 3; fcu < 40; (500/d)1/4 > 0.70 where tensile longitudinal steel ρw = As/bd (BS 5400-Part 4). Nominal concrete shear capacity, Vnominal = bd(ξsvc) (BS 5400-Part 4). Nominal shear links (if vs < 0.4 + vc) (BS 8110-Part 1:1997). Nominal shear links (if vs < ξsvc) (BS 5400-Part 4). Provide nominal shear links such that Asv/S > 0.4b/(fyv/γms) (BS 8110-Part 1:1997 and BS 5400-Part 4). Nominal concrete and links shear capacity, Vnominal = bd (vc + 0.4) (BS 8110-Part 1:1997). Nominal concrete and links shear capacity, Vnominal = bd (ξsvc + 0.4) (BS 5400-Part 4). For non-concentrated loads within 2d of support, design shear links (if vs > 0.4 + vc) (BS 8110-Part 1:1997) and design shear links (if vs > ξsvc) (BS 5400-Part 4). Provide stirrups such that Asv/S > b(vs-vc)/(fyv/γms) (BS 8110-Part 1:1997). Provide stirrups such that Asv/S > b(0.4+vs-ξsvc)/(fyv/γms) (BS 5400-Part 4). Provide longitudinal tensile reinforcement for shear (in excess of that for bending) i.e. Asa > V/(2(fy/γms)) (BS 5400-Part 4). For concentrated loads within 2d of support, enhanced shear capacity of concrete, vc,enhanced = 2dvc / av. Provide stirrups such that avAsv/S > avb(vs-vc,enhanced)/(fyv/γms) (BS 8110-Part 1:1997). Provide stirrups such that avAsv/S > avb(0.4+vs-ξsvc,enhanced)/(fyv/γms) (BS 5400-Part 4). Provide longitudinal tensile reinforcement for shear (in excess of that for bending) i.e. Asa > V/(2(fy/γms)) (BS 5400-Part 4). Design torsional links. Provide closed links such that Asv/S > T / (0.8x1y1(fyv/γms)) where horizontal dimension of closed link, x1 and vertical dimension of closed link, y1. Provide longitudinal bars evenly distributed round inside perimeter of links, As > (Asv/S)(fyv/fy)(x1+y1). Design shear and torsional links. Provide combined shear and torsion closed links such that Asv/S > (Asv/S)shear + (Asv/S)torsion. ULTIMATE LIMIT STATE DESIGN OF RECTANGULAR RC SECTION BS 8110-Part 1:1997 and BS5400-Part 4 1164 Structural Engineering Analysis and Design Second Edition Concrete and Steel Material Stress-Strain Curve Comments Units Characteristic Strength of Concrete fcu 50 Reference MPa Partial Safety Factor Steel, γms 1.15 Strength of shear link reinforcement steel, fyv 460 MPa Longitudinal torsion reinforcement steel, fy 460 MPa Section Dimensions 484 mm Width, b 1500 mm Area of Tensile Steel Reinforcement Provided, As 7238 mm2 Effective Depth, d Ultimate Shear Force To Be Resisted, V @ face of support 600 kN Design Shear Force To Be Resisted, V @ the critical section d (BS 8110) or 2d (BS 5400) 600 kN Torsional Moment To Be Resisted, T 0 kNm 0.83 MPa Design For Shear A. Ultimate Shear Stress To Be Resisted @ face of support Ultimate Shear Stress, vsupport = V / bd Check ultimate shear stress vsupport < Ultimate shear vu, lesser of 0.8(fcu)0.5 or 5 whichever smaller Check design shear stress vsupport < Ultimate shear vu, lesser of 0.75(fcu)0.5 or 4.75 whichever smaller OKCheck MPa BS 8110 OKCheck MPa BS 5400 B. Design Shear Stress vs To Be Resisted @ the critical section d (BS 8110) or 2d (BS 5400) Design Shear Stress, vs = V / bd 0.83 MPa C. Concrete Capacity 100As/bd Shear capacity of concrete, vc = (0.79/1.25)(100ρwfcu/25)1/3(400/d)1/4; 100ρw < 3; fcu < 40; (400/d)1/4 > 0.67 Shear capacity of concrete, vc = (0.79/1.25)(100ρwfcu/25)1/3(400/d)1/4; 100ρw < 3; fcu < 40; 1/4 (400/d) > 1.0 Shear capacity of concrete, ξsvc = (0.27/1.25)(100ρwfcu)1/3(500/d)1/4; 100ρw < 3; fcu < 40; (500/d)1/4 > 0.70 1.00 0.70Insufficient MPa BS 8110 0.74Insufficient BS 8110 0.74Insufficient MPa BS 5400 D. Nominal Links (BS8110: if vs < 0.4 + vc and BS5400: if vs < ζvc) Provide nominal links such that Asv / S > 0.4b/(fyv/γms) i.e. Asv / S > 1.50 mm2/mm BS 8110 & BS 5400 BS 8110 Nominal concrete shear capacity, Vnominal = bd (vc) 511 kN Nominal concrete shear capacity, Vnominal = bd (ξsvc) 540 kN BS 5400 Nominal concrete and links shear capacity, Vnominal = bd (0.4+vc) 802 kN BS 8110 Nominal concrete and links shear capacity, Vnominal = bd (0.4+ξsvc) 831 kN BS 5400 0.46 mm2/mm BS 8110 1.81 2 mm /mm BS 5400 750 2 mm BS 5400 500 mm2/m BS 5400 E. Design shear reinforcement (BS8110: if vs > 0.4 + vc and BS5400: if vs > ζvc) E (i) No concentrated load within 2d of support (Critical section d or 2d from face of support) Provide stirrups such that Asv / S > b(vs-vc)/(fyv/γms) i.e. Asv / S > Provide stirrups such that Asv / S > b(0.4+vs-ξcvc)/(fyv/γms) i.e. Asv / S > Provide longitudinal tensile reinforcement for shear (in excess of that for bending) i.e. Asa > V/(2(fy/γms)) Provide longitudinal tensile reinforcement for shear (in excess of that for bending) i.e. Asa/b > V/(2b(fy/γms)) Note that Asv is the cross sectional area of the stirrup * the number of stirrups Try:12 Diameter of 1 shear link Number of links in a cross section, i.e. number of legs 5 1165 mm Structural Engineering Analysis and Design Second Edition 565 mm2 Spacing, S (ensuring <0.75d and >80mm) 300OK mm Tried As / S value 1.88OK mm2/mm BS 8110 1.88OK 2 mm /mm BS 5400 N/A mm Area provided for shear resistance by all links in a cross-section, Asv Tried As / S value E (ii) Concentrated load within 2d of support, i.e. at av from support (Critical section av from face of support) av Enhanced shear capacity of concrete, vcenhanced = 2dvc / av #VALUE! MPa Provide stirrups such that av Asv / S > av b(vs-vcenhanced)/(fyv/γms) i.e. av Asv / S > #VALUE! mm2 BS 8110 #VALUE! 2 BS 5400 2 BS 5400 Provide stirrups such that avAsv / S > avb(0.4+vs-vcenhanced)/(fyv/γms) i.e. avAsv / S > Provide longitudinal tensile reinforcement for shear (in excess of that for bending) i.e. Asa > V/(2(fy/γms)) BS8110 requires this area of stirrups to be provided over the central three quarters of the shear span, av mm 750 mm Larger Dimension of Rectangular Section, hmax 1800 mm Smaller Dimension of Rectangular Section, hmin 850 mm Design Torsional Stress for Rectangular Sections, vt = 2T / ((hmin2)(hmax-hmin/3)) 0.00 MPa Wall thickness of thin hollow section, ht N/A mm Area enclosed by centre-line of thin hollow section, A N/A mm2 #VALUE! MPa Design For Torsion A. Maximum design torsion stress permissible Design Torsional Stress for Thin Hollow Section, vt = T / (2Aht) Design Torsional Stress for T-,L- or I-shaped divided into rectangular components and use T(hmin3 hmax)/ Σ(hmin3 hmax) 0.93 Design Torsional Stress, vt Check design torsion stresses vt < vu, lesser of 0.8(fcu)0.5 or 5 whichever smaller MPa OKCheck B. Design torsion reinforcement 670 mm Vertical dimension of closed link, y1 1605 mm Provide closed links such that Asv / S > T / (0.8x1y1(fyv/γms)) i.e. Asv / S > Provide longitudinal bars evenly distributed round inside perimeter of links, As > (Asv/S)(fyv/fy)(x1+y1) 0.00 mm2/mm Horizontal dimension of closed link, x1 2 0 mm Check design shear and torsion stresses vs + vt < vu, lesser of 0.8(fcu)0.5 or 5 whichever smaller 1.76OK MPa Provide combined shear and torsion closed links such that Asv / S > 0.46 mm /mm Design For Combined Shear and Torsion 2 Try:16 Diameter of 1 shear link mm 4 Number of links in a cross section, i.e. number of legs Area provided for shear resistance by all links in a cross-section, Asv 804 mm2 Spacing, S (ensuring <0.75d and >80mm) 300OK mm Tried As / S value 2.68OK mm2/mm 1166 Structural Engineering Analysis and Design Second Edition 8.4.2 Concepts of Moment Redistribution 1167 Structural Engineering Analysis and Design Second Edition 1168 Structural Engineering Analysis and Design Second Edition 1169 Structural Engineering Analysis and Design Second Edition 1170 Structural Engineering Analysis and Design Second Edition 1171 Structural Engineering Analysis and Design Second Edition 1172 Structural Engineering Analysis and Design Second Edition 1173 Structural Engineering Analysis and Design Second Edition 1174 Structural Engineering Analysis and Design Second Edition 1175 Structural Engineering Analysis and Design Second Edition 8.4.3 ULS Structural Floor Design – Reinforced Concrete 1176 Structural Engineering Analysis and Design Second Edition 8.4.4 ULS Structural Floor Design – Prestressed Concrete In office buildings, large spans are required. Pre- and post-tensioned floors are useful to maintain acceptable deflections without the need for expensive precambering. In residential buildings, large spans are not required as the tenant sees the space already subdivided by walls, which effectively hide the columns. Continuous spans can be achieved. However, unlike office buildings, residential buildings as a rule do not have suspended ceilings – the ceiling may just be sprayed high-build coating on the slab soffit or a plasterboard ceiling on battens fixed to the slab soffit. Flat-plate floors are therefore required and deflection control is an important design consideration, both achieved by pre- or post-tensioned floors. The major disadvantage of precast pre-tensioned floor beams or slabs is that the crainage required to lift the heavy units along with the field-welded connections required for stability and diaphragm action. Post-tensioned floors are usually more common for high-rise buildings. 8.4.4.1 (Precast) Pre-Tensioned 8.4.4.2 (Cast Insitu) Post-Tensioned Concrete Floor Systems Common post-tensioned systems are I. Post-tensioned flat slabs II. Post-tensioned beams supporting post-tensioned slabs III. Post-tensioned beams supporting RC slabs 1177 Structural Engineering Analysis and Design Second Edition 8.4.5 ULS Column Design – Bending, Axial, Shear and Torsion Effects 1178 Structural Engineering Analysis and Design Second Edition 8.4.6 ULS Wall Design 1179 Structural Engineering Analysis and Design Second Edition 8.4.7 ULS Connection Design 1180 Structural Engineering Analysis and Design Second Edition 8.4.8 ULS Fire Protection Design 1181 Structural Engineering Analysis and Design Second Edition 8.4.9 SLS Durability Design 1182 Structural Engineering Analysis and Design Second Edition 8.4.10 SLS Deflection Computation and Criteria 1183 Structural Engineering Analysis and Design Second Edition 1184 Structural Engineering Analysis and Design Second Edition 1185 Structural Engineering Analysis and Design Second Edition 1186 Structural Engineering Analysis and Design Second Edition 1187 Structural Engineering Analysis and Design Second Edition 1188 Structural Engineering Analysis and Design Second Edition 1189 Structural Engineering Analysis and Design Second Edition 1190 Structural Engineering Analysis and Design Second Edition 1191 Structural Engineering Analysis and Design Second Edition 1192 Structural Engineering Analysis and Design Second Edition 8.4.11 SLS Crack Width Calculations 1193 Structural Engineering Analysis and Design Second Edition 8.5 Prestressed Concrete Analysis and Design 1194 Structural Engineering Analysis and Design Second Edition 1195 Structural Engineering Analysis and Design Second Edition 1196 Structural Engineering Analysis and Design Second Edition 1197 Structural Engineering Analysis and Design Second Edition 1198 Structural Engineering Analysis and Design Second Edition 1199 Structural Engineering Analysis and Design Second Edition 1200 Structural Engineering Analysis and Design Second Edition 1201 Structural Engineering Analysis and Design Second Edition 1202 Structural Engineering Analysis and Design Second Edition 1203 Structural Engineering Analysis and Design Second Edition 1204 Structural Engineering Analysis and Design Second Edition 1205 Structural Engineering Analysis and Design Second Edition 1206 Structural Engineering Analysis and Design Second Edition 1207 Structural Engineering Analysis and Design Second Edition 1208 Structural Engineering Analysis and Design Second Edition 1209 Structural Engineering Analysis and Design Second Edition 1210 Structural Engineering Analysis and Design Second Edition 1211 Structural Engineering Analysis and Design Second Edition 1212 Structural Engineering Analysis and Design Second Edition 1213 Structural Engineering Analysis and Design Second Edition 1214 Structural Engineering Analysis and Design Second Edition 1215 Structural Engineering Analysis and Design Second Edition 1216 Structural Engineering Analysis and Design Second Edition 1217 Structural Engineering Analysis and Design Second Edition 1218 Structural Engineering Analysis and Design Second Edition 1219 Structural Engineering Analysis and Design Second Edition 1220 Structural Engineering Analysis and Design Second Edition 1221 Structural Engineering Analysis and Design Second Edition 1222 Structural Engineering Analysis and Design Second Edition 1223 Structural Engineering Analysis and Design Second Edition 1224 Structural Engineering Analysis and Design Second Edition 1225 Structural Engineering Analysis and Design Second Edition 1226 Structural Engineering Analysis and Design Second Edition 1227 Structural Engineering Analysis and Design Second Edition 1228 Structural Engineering Analysis and Design Second Edition 1229 Structural Engineering Analysis and Design Second Edition 1230 Structural Engineering Analysis and Design Second Edition 1231 Structural Engineering Analysis and Design Second Edition 1232 Structural Engineering Analysis and Design Second Edition 1233 Structural Engineering Analysis and Design Second Edition 1234 Structural Engineering Analysis and Design Second Edition 1235 Structural Engineering Analysis and Design Second Edition 1236 Structural Engineering Analysis and Design Second Edition 1237 Structural Engineering Analysis and Design Second Edition 1238 Structural Engineering Analysis and Design Second Edition 1239 Structural Engineering Analysis and Design Second Edition 1240 Structural Engineering Analysis and Design Second Edition 1241 Structural Engineering Analysis and Design Second Edition 1242 Structural Engineering Analysis and Design Second Edition 1243 Structural Engineering Analysis and Design Second Edition 8.6 8.6.1 Steel Design to BS 5950-Part 1:2000 (Buildings) ULS Beam and Column Design – Bending (Incorporating High Shear Effects), Axial, Shear and Buckling Effects BS 5950-Part 1:2000 gives steel design strength based on thickness as follows. Note that the material partial safety factor is 1.0. Steel castings and forgings may be used for components in bearings, junctions and other similar parts. Castings should conform to BS 3100 and forgings should conform to BS EN 10250-2. Unless better information is available, design strengths corresponding to structural steel grade S 275 may be adopted. To obtain the moment capacity (cl. 4.2.5), the following procedure is undertaken. The cross is classified to account for plate buckling as described in Section 3.2.5.1.3. Note that additional considerations to moment capacity must be made according to cl. 4.4.4.2 if web is subject to shear buckling as described in Section 3.2.5.1.4. For low shear force, i.e. if Fv < 0.6Pv, then Mc = pyS < 1.2Zpy for Class 1 plastic or Class 2 compact cross sections pyZ for Class 3 semi-compact cross sections pyZeff for Class 4 slender cross sections For high shear force, i.e. if Fv > 0.6Pv, then Mc = py(S-ρSv) < 1.2Zpy for Class 1 plastic or Class 2 compact cross sections py(Z-ρSv/1.5) for Class 3 semi-compact cross sections py(Zeff-ρSv/1.5) for Class 4 slender cross sections in which Sv is for sections with unequal flanges Sv = S – Sf where Sf is the plastic modulus of the effective section excluding the shear area Av, or for other sections Sv is the plastic modulus of the shear area Av and ρ is given by [2(Fv/Pv) – 1]2. 1244 Structural Engineering Analysis and Design Second Edition Alternatively, for symmetrical sections, the following simplified formula may be used for high shear force, i.e. if Fv > 0.6Pv where D is the total depth and t is the web thickness. Clearly, a reduction in the moment capacity is incorporated to reduce the contribution of the web in circumstances where it is highly stressed from the shear force. Note that to avoid irreversible deformation under serviceability loads, the value of the moment capacity Mc should be limited to 1.5pyZ generally and to 1.2pyZ in the case of a simply supported beam or a cantilever. The moment capacity, Mc is calculated differently if the I-, H- or channel section is notched at its ends. The elastic section modulus Z of the remaining unnotched section is used in the calculation and is described in cl. 4.2.5.4. The section capacity (for Class 1, 2 or 3 sections) under moment and axial (tension or compression) forces must be checked according to the following (cl. 4.8.2.2 or cl. 4.8.3.2) Ensure utilisation = My Mx F + + ≤1 Ap y S x p y S y p y The shear force Fv should not be greater than the shear capacity Pv given by (cl. 4.2.3) where the shear area of the web of an I- section, Av = tD, t the web thickness and D the overall depth of section. If the section is a plate girder (i.e. welded), then the shear area is td where d is the web depth. Elements are checked for Perry-Robertson buckling (Section 3.1.6.6.1), secant buckling (Section 3.1.6.6.2), lateral-torsional buckling (Section 3.1.6.6.3) and a combination of buckling (Section 3.1.6.6.4). 1245 Structural Engineering Analysis and Design Second Edition 8.6.2 ULS Plate Girder Beam and Column Design – Bending (Incorporating High Shear Effects), Axial, Shear and Buckling Effects Plate girders are used when beams are required to resist forces and bending moments much higher than that which can be resisted by standard rolled sections. A plastic design methodology is used. For best performance, the web flange weld should be continuous and made by an automatic process. Intermittent welds give low fatigue strength. Assuming a few section shape limitations (i.e. that the section is at least compact) are satisfied, a plate girder can be conservatively designed almost in the same way as a normal rolled section (Section 8.6.1). Span to depth ratio of (non-composite) simply-supported plate girders are 10 to 15 and (non-composite) continuous plate girders are 15 to 20. 1246 Structural Engineering Analysis and Design Second Edition 8.6.3 ULS Structural Floor Design – Composite Steel and Reinforced Concrete 8.6.3.1 Floor Framing Composite floor systems typically involve simply supported structural steel beams, girders or trusses linked via shear connectors with a concrete floor slab to form an effective T-beam flexural member resisting primarily gravity loads. The versatility of the system stems from the inherent strength of the concrete floor component in compression and the tensile strength and spannability of the steel member. The slab and beam arrangement also produces a rigid horizontal diaphragm, providing stability to the overall building system while distributing wind and seismic shears to the lateral load resisting system elements. Consideration must be given to the floor layout. Primary beams span between column or other predetermined supports. Secondary beams are then required if floors are unable to span between primary beams. Below is shown an inefficient and efficient flooring arrangements, i.e. the primary beams should span the shorter dimension whilst the secondary beam spans the longer dimension to keep overall depths to a minimum. The spacing between the secondary beams are governed by the span capability of the concrete floor, usually about 3m for no propping during construction. 1247 Structural Engineering Analysis and Design Second Edition 8.6.3.2 Simple Steel I-Beam With Non-Composite or Composite Precast (Hollow) Slabs These proprietary products can act compositely or not. If hollow, and to act compositely, then the effective width may have to be reduced according to the manufacturer recommendations. 8.6.3.3 Prismatic Steel I-Beam Encased in T-section Reinforced Concrete, Flat Part of the T- Above the Top Flange of I-Beam This is an old solution before the advent of sprayed-on fire-proofing. 8.6.3.4 Prismatic Steel I-Beam Shear Studded Into Flat-Soffit Reinforced Concrete Slab 1248 Structural Engineering Analysis and Design Second Edition 8.6.3.5 Prismatic Steel I-Beam Shear Studded Into (Parallel Or Perpendicular Ribbed) Metal Deck With Reinforced Concrete 1249 Structural Engineering Analysis and Design Second Edition 8.6.3.6 Prismatic Steel Plate Girder Shear Studded into Flat-Soffit Reinforced Concrete or (Parallel or Perpendicular Ribbed) Metal Deck with Reinforced Concrete Assuming a few section shape limitations and properties are satisfied (Section 8.6.2), a plate girder can be conservatively designed almost in the same way as a normal rolled section, in which case the composite plate girder with metal decking and reinforced concrete floor can also be designed as if the plate girder is a standard rolled section (Section 8.6.3.5). Span to depth ratio of simply-supported composite plate girders are 12 to 20. 8.6.3.7 Prismatic Steel I-Beam With Stub Girder And Reinforced Concrete Slab 1250 Structural Engineering Analysis and Design Second Edition 8.6.3.8 Prismatic Steel I-Beam With Web Openings, Castellated Beam, Cellular Beam or Westok Beam Shear Studded into Flat-Soffit Reinforced Concrete or (Parallel or Perpendicular Ribbed) Metal Deck with Reinforced Concrete These have the advantage of increased spanability and stiffness due to the deeper structural depth and ease in accommodating electrical conduits, plumbing pipes and hearing and air-conditioning ductwork. Openings in the web can be up to 70% and can be rectangular or circular in shape. At failure of beams with web openings, all the elements around the web are subject to high combined stresses generated by axial forces from global bending, shear forces and also now additional local moments arising from the Vierendeel action. 1251 Structural Engineering Analysis and Design Second Edition Castellated sections are not very good for point loads. Span to depth must be < 20. Even if the guidelines are followed, beams with web openings must still be checked for its capacity taking into account the Vierendeel moments. Checks are based on web openings in composite and non-composite beams (SCI Publications 068). 1252 Structural Engineering Analysis and Design Second Edition 1253 Structural Engineering Analysis and Design Second Edition 1254 Structural Engineering Analysis and Design Second Edition 1255 Structural Engineering Analysis and Design Second Edition 1256 Structural Engineering Analysis and Design Second Edition 1257 Structural Engineering Analysis and Design Second Edition 8.6.3.9 Prismatic Steel Warren (or Modified Warren) Truss or Pratt Truss, Both With or Without a Vierendeel Panel in the Middle (for the Main Mechanical Duct) Shear Studded into Flat-Soffit Reinforced Concrete or (Parallel or Perpendicular Ribbed) Metal Deck with Reinforced Concrete These have the advantage of increased spanability and stiffness due to the deeper structural depth and ease in accommodating electrical conduits, plumbing pipes and hearing and air-conditioning ductwork. Open web systems however carry the premium for fire-proofing the many, relatively thin, components of the member. 8.6.3.10 Nonprismatic Tapered (Shallower at the Supports) Steel Plate Girder Shear Studded Into (Parallel or Perpendicular Ribbed) Metal Deck with Reinforced Concrete A prismatic composite steel beam has two fundamental disadvantages. Firstly, the simply-supported member must be designed for maximum bending moment near the midspan and thus is often understressed near the supports, and secondly building services ductwork and piping must pass beneath the beam or the beam must be provided with web penetrations (normally reinforced with plates or angles leading to higher fabrication costs) to allow access for equipment. As the non-prismatic tapered girder is completely fabricated from plate elements or cut from rolled shapes, these composite members are frequently hybrid, with the top flange designed in lower strength steel. However, a relatively wide and thick-gauge top flange must be provided for proper and effective shear stud installation. 1258 Structural Engineering Analysis and Design Second Edition 8.6.4 ULS Composite Column Design 1259 Structural Engineering Analysis and Design Second Edition 8.6.5 ULS Connection Design 1260 Structural Engineering Analysis and Design Second Edition 8.6.6 ULS Bearing and Joints Design 1261 Structural Engineering Analysis and Design Second Edition 8.6.7 ULS Brittle Fracture Design Brittle fracture is described in Section 6.3.28.2.2. 8.6.8 ULS Fatigue Design Fatigue design is described in Section 5.5. 1262 Structural Engineering Analysis and Design Second Edition 8.6.9 ULS Fire Protection Design Steel performs badly in fire. Temperatures reach 1200°C at the seat of the fire while the critical temperature for steel is about 550°C, when the yield stress of steel has fallen to 0.7 of its value at ambient temperatures. In general choose 1h fire protection for superstructure and 2h for ground floor and basement structure. 1263 Structural Engineering Analysis and Design Second Edition 1264 Structural Engineering Analysis and Design Second Edition 8.6.10 SLS Human Induced Vibration Human footfall induced vibrations are described in Section 5.2. 1265 Structural Engineering Analysis and Design Second Edition 8.6.11 SLS Deflection Criteria BS 5950-Part 1:2000 gives suggested limits for calculated static deflections for the live load serviceability limit state (SLS). Note that only unfactored imposed (live) loads are required. For multi-storey buildings a limit of storey height/500 may be more appropriate where the cladding cannot accommodate greater movement. 1266 Structural Engineering Analysis and Design Second Edition 1267 Structural Engineering Analysis and Design Second Edition 8.6.12 SLS Corrosion Protection Surface preparation is the most important single factor in achieving successful protection against corrosion. All rolled steel are covered with a thin layer of iron oxide called mill scale which must be removed before corrosion protection is applied as it will break off under flexure or abrasion and expose the steel to rusting. Surface preparation can be performed by manual cleaning using scrapers, flame cleaning using a torch, pickling in a tank of acid used as a preparation for galvanizing or blast cleaning where iron grit or sand is projected against the steel surface. Protective coatings used are usually metal spraying (using zinc and aluminium coatings) and galvanizing or paint systems. Some general guidance for multi-storey steel buildings in non-polluted inland sites is presented. Some common schemes are presented. 1268 Structural Engineering Analysis and Design Second Edition 1269 Structural Engineering Analysis and Design Second Edition 8.7 Steel Design to BS 5400-Part 3 (Bridges) BS 5400-Part 3 is generally based upon elastic design methodology, unlike BS 5950-Part 1 which is based upon the plastic design methodology. 1270 Structural Engineering Analysis and Design Second Edition 8.8 Timber Design to EC5 Conceptually, in EC5 and BS 5268, element design is based on elastic design and not plastic design. In EC5, the ULS (i.e. factored) loads are used. This is unlike BS 5268 which is based on working (i.e. unfactored) loads. The material properties i.e. Young’s Modulus, shear modulus, density and strength depends on the strength class. Note that the shear modulus, G is not E/2/(1+ν) as the timber beams are orthotropic. Hence in the modelling of linear elastic beam elements for structural analysis, E, G and ν must be explicitly input to model the orthotropic property. Another significant point is that the design strength of timber varies for permanent, long-term, medium-term, short-term and instantaneous loads due to the dependency of the design parameter kmod for loading of different durations. This means that the ULS combination of 1.35Dead + 1.35SDL + γpPrestress + 1.5Livei +1.5ψ0Liveother i must be checked independently for the timber-specific time duration dependent loading. For instance, for the ULS factored permanent structure self weight and ULS factored permanent partitions live loading combination, a value of kmod of 0.6 (assuming service class 2) is used. Then, for the ULS factored structure self weight, ULS factored permanent partitions live load and ULS factored short-term wind and ULS factored snow live loading combination, a value of kmod of 0.9 (assuming service class 2) is used. Also, the structural analyses that are performed to obtain the effects for these permanent and short-term cases are also necessarily based upon stiffness values (Young’s modulus E and shear modulus G) which are different (to account for effects of creep and moisture), the difference characterized by the parameter kdef. These properties for permanent action and short term action are illustrated in the following example for the Centre Pompidou, Metz. A Permanent Action A.1 Properties for Linear Structural Analysis kdef,perm = 0.8 E = Emean / (1+kdef,perm) = 13.5GPa / 1.8 = 7.50GPa G = Gmean / (1+kdef,perm) = 0.56GPa / 1.8 = 0.31GPa A.2 ULS Loading and Simplified Combined Axial and Bending Stress Capacity Check For permanent action, the load case is the factored permanent loads. Hence French combinations 1.35(DL) + 1.35(SDL) The combined axial and bending stresses are checked against the design ultimate strength. kmod,perm = 0.6 γm = 1.2 ft/c,0,d = (kmod,perm / γm)ft/c,0,k = (0.6/1.2) x 37MPa = 18.5MPa The higher bending strength cannot be used unless the only effects are bending, i.e. no axial. A.3 SLS Loading and Deflection Check For permanent action, the load case is the unfactored permanent loads. Hence French combinations 1.0(DL) + 1.0(SDL) These deflections are checked against acceptable deflection criteria. 1271 Structural Engineering Analysis and Design Second Edition B Short Term Action B.1 Properties for Linear Structural Analysis kdef,st = 0.0 ψ2,st = 0.2 E = Emean / (1+ψ2,stkdef,st) = 13.5GPa / 1.0 = 13.5GPa G = Gmean / (1+ψ2,stkdef,st) = 0.56GPa / 1.0 = 0.56GPa B.2 ULS Loading and Simplified Combined Axial and Bending Stress Capacity Check For short term action, the load case is the factored short term loads. Hence French combinations 1.35(DL) + 1.35(SDL) + 1.5(Wind) 1.35(DL) + 1.35(SDL) + 1.5(Snow) 1.35(DL) + 1.35(SDL) + 1.35(Wind) + 1.35(Snow) The combined axial and bending stresses are checked against the design ultimate strength. kmod,st = 0.9 γm = 1.2 ft/c,0,d = (kmod,st / γm)ft/c,0,k = (0.9/1.2) x 37MPa = 27.75MPa The higher bending strength cannot be used unless the only effects are bending, i.e. no axial. B.3 SLS Loading and Deflection Check For short term action, the load case is the unfactored short term loads. The result from the permanent load action (which is based on different creep dependent stiffness values) is added to the short term loads. Hence French combinations Results A.3 + 1.0(Wind) Results A.3 + 1.0(Snow) Results A.3 + 1.0(Wind) + 1.0(Snow) These deflections are checked against acceptable deflection criteria. 1272 Structural Engineering Analysis and Design Second Edition 8.8.1 ULS Beam and Column Design 1273 Structural Engineering Analysis and Design Second Edition 8.8.2 ULS Dowel (Nailed, Screwed, Bolted, Doweled) Connection Design Generally there are 4 types of connections in timber, namely direct bearing (most efficient), glued joints (scarf joints, finger joints, and occasionally glued in fin-plates), dowels (including nails, screws, bolts, dowels) and timber connectors (split rings, shear plates and toothed connectors). 1274 Structural Engineering Analysis and Design Second Edition 8.8.3 ULS Fire Protection Design The rate of charring is about 0.6mm/minute and so to provide 30 minutes fire protection, a member would need to be 20mm larger on all exposed faces. 1275 Structural Engineering Analysis and Design Second Edition 8.9 Masonry Design to BS 5628 Typical material properties are presented. Fire protection requirements are presented. 1276 Structural Engineering Analysis and Design Second Edition 9 GEOTECHNICAL ENGINEERING 9.1 Basic Soil Mechanics 1277 Structural Engineering Analysis and Design Second Edition 1278 Structural Engineering Analysis and Design Second Edition 1279 Structural Engineering Analysis and Design Second Edition 1280 Structural Engineering Analysis and Design Second Edition 1281 Structural Engineering Analysis and Design Second Edition 1282 Structural Engineering Analysis and Design Second Edition 1283 Structural Engineering Analysis and Design Second Edition 9.2 Slope Stability Analysis 1284 Structural Engineering Analysis and Design Second Edition 1285 Structural Engineering Analysis and Design Second Edition 1286 Structural Engineering Analysis and Design Second Edition 1287 Structural Engineering Analysis and Design Second Edition 9.3 Earth Pressure Analysis and Retaining Wall Design 1288 Structural Engineering Analysis and Design Second Edition 1289 Structural Engineering Analysis and Design Second Edition 1290 Structural Engineering Analysis and Design Second Edition 1291 Structural Engineering Analysis and Design Second Edition 1292 Structural Engineering Analysis and Design Second Edition 1293 Structural Engineering Analysis and Design Second Edition 1294 Structural Engineering Analysis and Design Second Edition 1295 Structural Engineering Analysis and Design Second Edition 1296 Structural Engineering Analysis and Design Second Edition 1297 Structural Engineering Analysis and Design Second Edition 1298 Structural Engineering Analysis and Design Second Edition 1299 Structural Engineering Analysis and Design Second Edition 1300 Structural Engineering Analysis and Design Second Edition 1301 Structural Engineering Analysis and Design Second Edition 1302 Structural Engineering Analysis and Design Second Edition 1303 Structural Engineering Analysis and Design Second Edition 1304 Structural Engineering Analysis and Design Second Edition 1305 Structural Engineering Analysis and Design Second Edition 1306 Structural Engineering Analysis and Design Second Edition 1307 Structural Engineering Analysis and Design Second Edition 1308 Structural Engineering Analysis and Design Second Edition 1309 Structural Engineering Analysis and Design Second Edition 1310 Structural Engineering Analysis and Design Second Edition 1311 Structural Engineering Analysis and Design Second Edition 9.4 9.4.1 Foundation Design Scheme Design 1312 Structural Engineering Analysis and Design Second Edition 1313 Structural Engineering Analysis and Design Second Edition 1314 Structural Engineering Analysis and Design Second Edition 1315 Structural Engineering Analysis and Design Second Edition 9.4.2 Allowable Bearing Pressure 1316 Structural Engineering Analysis and Design Second Edition 1317 Structural Engineering Analysis and Design Second Edition 9.4.3 Pad Footing Pad footings are used under individual columns. 1318 Structural Engineering Analysis and Design Second Edition 1319 Structural Engineering Analysis and Design Second Edition 1320 Structural Engineering Analysis and Design Second Edition 1321 Structural Engineering Analysis and Design Second Edition 1322 Structural Engineering Analysis and Design Second Edition 1323 Structural Engineering Analysis and Design Second Edition 1324 Structural Engineering Analysis and Design Second Edition 1325 Structural Engineering Analysis and Design Second Edition 1326 Structural Engineering Analysis and Design Second Edition 1327 Structural Engineering Analysis and Design Second Edition 1328 Structural Engineering Analysis and Design Second Edition 9.4.4 Strip Footing Strip footings are used under walls or a row of columns. 1329 Structural Engineering Analysis and Design Second Edition 9.4.5 Raft Foundation Raft foundations are large slabs which support the complete building. 1330 Structural Engineering Analysis and Design Second Edition 9.4.6 Basement Foundation Basements can be of one or more stories and form an underground extension to the building that often serves as a carpark. 1331 Structural Engineering Analysis and Design Second Edition 1332 Structural Engineering Analysis and Design Second Edition 1333 Structural Engineering Analysis and Design Second Edition 1334 Structural Engineering Analysis and Design Second Edition 1335 Structural Engineering Analysis and Design Second Edition 9.4.7 Piled Foundation Piled foundations can be used in combination with other foundations types which function as the pile cap. 1336 Structural Engineering Analysis and Design Second Edition 1337 Structural Engineering Analysis and Design Second Edition 1338 Structural Engineering Analysis and Design Second Edition 1339 Structural Engineering Analysis and Design Second Edition Approximate pile design for London clay is presented. 1340 Structural Engineering Analysis and Design Second Edition 9.5 Settlement Analysis 1341 Structural Engineering Analysis and Design Second Edition 1342 Structural Engineering Analysis and Design Second Edition 1343 Structural Engineering Analysis and Design Second Edition 1344 Structural Engineering Analysis and Design Second Edition 1345 Structural Engineering Analysis and Design Second Edition 1346 Structural Engineering Analysis and Design Second Edition 1347 Structural Engineering Analysis and Design Second Edition 10 CONVERSION FACTORS 1348 Structural Engineering Analysis and Design Second Edition BIBLIOGRAPHY Structural Analysis and Mechanics of Materials 1. 2. 3. 4. 5. 6. 7. 8. 9. 10. BALFOUR, James A.D. Computer Analysis of Structural Frameworks 2nd Edition. Blackwell Scientific Publications, Oxford, 1992. BHATT, P. Structures. Longman, England, 1999. GAY, Daniel, HOA, Suong, TSAI, Stephen. Composite Materials Design and Application. CRC Press, London, 2003. CIDECT. Design Guide For Rectangular Hollow Sections (RHS) Joints Under Predominantly Static Loading. Rheinland, Germany, 1992. TIMOSHENKO & GERE. Mechanics of Materials 4th SI Edition. Stanley Thornes, United Kingdom, 1991. BUDYNAS, Richard. Advanced Strength and Applied Stress Analysis Second Edition. McGraw-Hill International, Singapore, 1999. ROARK, R.J. and YOUNG, W.C. Roark’s Formulas for Stress and Strain 7th Edition. McGraw-Hill, London. MCEVILY, Arthur, J. Metal Failures, Mechanisms, Analysis, Prevention. John Wiley & Sons, New York, 2002. LEVY, Matthys and SALVADORI, Mario. Why Buildings Fall Down. W.W. Norton & Company Ltd., United States of America, 1992. CONCRETE SOCIETY. Design Guidance for Strengthening Concrete Structures Using Fibre Composite Materials. Technical Report 55, The Concrete Society, United Kingdom, 2000. Finite Element Theory 11. 12. 13. 14. 15. ZIENKIEWICZ, O.C. & TAYLOR, R.L. The Finite Element Method. The Basis. Volume 1. 5th Edition. Butterworth-Heinemann, Oxford, 2000. COOK, Robert; MALKUS, David; PLESHA, Michael; WITT, Robert; Concepts & Applications of Finite Element Analysis Fourth Edition. John Wiley & Sons, Inc, United States of America, 2002. FELIPPA, Carlos A. Introduction to Finite Element Methods. Center for Aerospace Structures, University of Colorado, 2001. FELIPPA, Carlos A. Advanced Finite Element Methods. Center for Aerospace Structures, University of Colorado, 2001. FELIPPA, Carlos A. Nonlinear Finite Element Methods. Center for Aerospace Structures, University of Colorado, 2001. Finite Element Modelling 16. 17. 18. 19. NAFEMS. A Finite Element Primer. NAFEMS Ltd., Great Britain, 1992. ADAMS, Vince. Building Better Products With Finite Element Analysis. High Mountain Press, 1999. SPYRAKOS, Constantine. Finite Element Modelling In Engineering Practice. West Virginia University Press, United States of America, 1994. HITCHINGS, Dennis. A Finite Element Dynamics Primer. NAFEMS Ltd., Great Britain, September 1991. Dynamics 20. 21. 22. 23. HARTOG, Den J.P. Mechanical Vibrations 4th Edition. McGraw-Hill Book Co., New York, 1934. PAZ, Mario. Structural Dynamics Theory and Computation. Chapman and Hall, New York, 1997. SPENCE, Dr. Peter. What is ‘Power Spectral Density’. The Analyst. WHITTAKER, Andrew. Introduction to Earthquake Engineering Lecture Notes. University of Buffalo, 2001. 1349 Structural Engineering Analysis and Design Second Edition 24. 25. 26. 27. 28. 29. 30. 31. 32. 33. 34. 35. 36. SADEK, Fahim et al. A Method Of Estimating The Parameters of Tuned Mass Dampers For Seismic Applications. John Wiley & Sons Ltd., Earthquake Engineering and Structural Dynamics, Vol 26, 617-635, 1997. CONNOR, Jerome. Introduction to Structural Motion Control. Prentice Hall, Massachusetts Institute of Technology, 2003. BACHMANN, Hugo. Vibration Problems in Structures Practical Guidelines. Birkhauser, Berlin, 1995. DESIGN MANUAL FOR ROADS AND BRIDGES. Design Rules for Aerodynamic Effects on Roads and Bridges BD 49/01. Highways Agency, UK. TRL Limited. Background to the Development of BD 49/01: Design Rules for Aerodynamic Effects on Roads and Bridges BD 49/01. TRL Report 528, TRL Limited, United Kingdom, 2002. EWINS, D.J. Modal Testing Theory, Practice and Application Second Edition. Research Studies Press Ltd, England, 2000. JIMIN, He and ZHI-FANG, Fu. Modal Analysis. Butterworth-Heinemann, Great Britain, 2001. BRUEL & KJAER. Vibration Analysis, Measurement and Testing. Denmark, 2001. CLOUGH R.W. & PENZIEN J. Dynamics of Structures 2nd Edition. McGraw-Hill Book Co., United States, 1993. SMITH, J.W. Vibration of Structures, Application in Civil Engineering Design. Chapman and Hall, London, 1988. BEARDS, C. F. Structural Vibration Analysis, Modelling, Analysis and Damping in Vibrating Structures. Ellis Horwood, London, 1983. SELVAM, Dr. R.P & GOVINDASWAMY, Suresh. Aeroelastic Analysis of Bridge Girder Section Using Computer Modelling. University of Arkansas, May 2001. SIMIU and SCALAN. Wind Effects on Structures, An Introduction to Wind Engineering. Imperial College of Science, Technology and Medicine, London 37. 38. 39. 40. 41. 42. 43. 44. 45. 46. 47. 48. 49. Dr IZZUDDIN, Bassam. Non-Linear Structural Mechanics. Imperial College of Science Technology and Medicine, London, 2000. Dr IZZUDDIN, Bassam. Computational Engineering Analysis MEng Lectures. Imperial College of Science Technology and Medicine, London, 1999. Dr WADEE, M. Structural Stability Systems Lecture Notes. Imperial College of Science Technology and Medicine, London, 2000. Dr LLYOD, Smith. Plastic Collapse Analysis Lectures. Imperial College of Science Technology and Medicine, London, 2000. Dr LLYOD, Smith. Aerodynamic Forces on Structures. Imperial College of Science Technology and Medicine, London, 2000. Prof HOBBS. Virtual Work, Flexibility, Direct Stiffness Method, and Moment Distribution Method Lectures. Imperial College of Science Technology and Medicine, London, 1999. Dr BOMMER, Earthquake Engineering Seismicity Lectures. Imperial College of Science Technology and Medicine, London, 2001. Dr SARMA, Earthquake Engineering Soil Effects Lectures. Imperial College of Science Technology and Medicine, London, 2001. Prof ELNASHAI, Earthquake Engineering Seismic Analysis Lectures. Imperial College of Science Technology and Medicine, London, 2001. Dr PINHO. Earthquake Engineering RC Detailing Lectures. Imperial College of Science Technology and Medicine, London, 2001. Dr SWAN. Wave Mechanics and Wave Loading Lectures. Imperial College of Science Technology and Medicine, London, 2000. Dr RAMACHANDRAN, K. Structural Dynamics College Lectures. Imperial College of Science Technology and Medicine, London, 2001. Dr Hardwick, J.D. Fluid Mechanics Lectures. Imperial College of Science Technology and Medicine, London, 1997-1998. 1350 Structural Engineering Analysis and Design Second Edition 50. 51. 52. Prof WYATT, Tom. Steel Design MEng 4th Year. Imperial College of Science Technology and Medicine, London, 2001. Dr ELGHAZOULI. Steel Design. Imperial College of Science Technology and Medicine, London, 1999. Dr IZZUDDIN, Bassam. Computational Engineering Analysis MSC Lectures. Imperial College of Science Technology and Medicine, London, 1999. MacNeal-Schwendler Corporation 53. 54. 55. 56. 57. 58. 59. 60. 61. 62. 63. 64. 65. 66. 67. 68. 69. 70. 71. 72. 73. 74. SITTON, Grant. MSC.NASTRAN Basic Dynamic Analysis User’s Guide. The MacNeal-Schwendler Corporation, Los Angeles, U.S.A, July 1997. MOORE, Gregory J. MSC.NASTRAN Design Sensitivity and Optimization User’s Guide. The MacNealSchwendler Corporation, U.S.A, 1995. KOMZSIK, Louis. MSC.NASTRAN Numerical Methods User’s Guide. The MacNeal-Schwendler Corporation, U.S.A, 1998. MILLER, Mark. Getting Started With MSC.NASTRAN User’s Guide. 2nd Edition. The MacNeal-Schwendler Corporation, U.S.A, 1996. MACNEAL-SCHWENDLER CORP. MSC.NASTRAN Practical Dynamic Analysis Seminar Notes. BISHOP, Dr. Neil. Fundamentals of FEA Based Fatigue Analysis & Vibration Fatigue in MSC.FATIGUE and MSC.NASTRAN Seminar Notes 2002. MacNeal-Schwendler Corp., England, 2002. LEE, John. MSC.NASTRAN Linear Static Analysis User’s Guide Version 69. The MacNeal-Schwendler Corporation, U.S.A, May 1997. MATINEZ, Angel. Submodelling Techniques for Static Analysis. MSC. Software First South European Technology Conference, 7-9 June 2000. LEE, John M. MSC.NASTRAN Common Questions and Answers. 3rd Edition. The MacNeal-Schwendler Corporation, U.S.A, 1997. DICKENS, J, NAKAGAWA, J, WITTBRODT. A Critique of Mode Acceleration And Modal Truncation Augmentation Methods For Modal Response Analysis. Elsevier Science Ltd., Computers and Structures Volume 62, No. 6, 1997. MACNEAL-SCHWENDLER CORP. MSC.NASTRAN Nonlinear Analysis Seminar Notes. MacNealSchwendler Corp., Los Angeles, May 1994. MACNEAL-SCHWENDLER CORP. MSC.NASTRAN Reference Manual 2001. MacNeal-Schwendler Corp., Los Angeles, 2001. MACNEAL-SCHWENDLER CORP. MSC.NASTRAN Release Guide 70.7. The MacNeal-Schwendler Corporation, U.S.A. MACNEAL-SCHWENDLER CORP. MSC.NASTRAN Release Guide 2001. The MacNeal-Schwendler Corporation, U.S.A, 2001. MACNEAL-SCHWENDLER CORP. MSC.NASTRAN Release Guide 2004. The MacNeal-Schwendler Corporation, U.S.A, 2004. HERTING, David. MSC.NASTRAN Advanced Dynamic Analysis User’s Guide. The MacNeal-Schwendler Corporation, U.S.A, 1997. MACNEAL-SCHWENDLER CORP. MSC.NASTRAN Practical Finite Element Modelling Techniques Seminar Notes. BELLINGER, Dean. Dynamic Analysis by the Fourier Transform Method with MSC.NASTRAN. MacNealSchwendler Corp., Los Angeles, 1995. MACNEAL-SCHWENDLER CORP. MSC.NASTRAN Fatigue Analysis Quick Start Guide 2001. MacNealSchwendler Corp., Los Angeles, 2001. MACNEAL-SCHWENDLER CORP. MSC.NASTRAN Fatigue Analysis User Guide 2001. MacNealSchwendler Corp., Los Angeles, 2001. MACNEAL-SCHWENDLER CORP. MSC.NASTRAN Aeroelastic Analysis User Guide 2001. MacNealSchwendler Corp., Los Angeles, 2001. MACNEAL-SCHWENDLER CORP. MSC.NASTRAN Superelement User’s Guide 2001. The MacNealSchwendler Corporation, U.S.A, 2001. 1351 Structural Engineering Analysis and Design Second Edition 75. MACNEAL-SCHWENDLER CORP. MSC 1995 World User’s Conference Proceedings. MacNealSchwendler Corp., Los Angeles, 1995. Livermore Software Technology Corporation 76. 77. LIVERMORE SOFTWARE TECHNOLOGY CORPORATION. LS-DYNA Keyword User’s Manual Version 950. Livermore Software Technology Corporation, California, U.S.A, May 1999. LIVERMORE SOFTWARE TECHNOLOGY CORPORATION. LS-DYNA Theoretical Manual Version 950. Livermore Software Technology Corporation, California, U.S.A, May 1999. Ove Arup & Partners International Ltd 78. 79. 80. 81. 82. 83. 84. 85. 86. 87. 88. 89. 90. 91. 92. 93. 94. 95. 96. IZATT, Conrad. Dynamic Relaxation in LS-DYNA. Advanced Technology Ove Arup & Partners International Ltd., London. HARGREAVES, James. Modal Analysis, Forced Response And Optimization In MSC.NASTRAN For Vehicle NVH Applications. Advanced Technology Ove Arup & Partners International Ltd., Coventry, 1998. HARGREAVES, James. Introduction to MSC.NASTRAN Training for ATG Graduates. Advanced Technology Ove Arup & Partners International Ltd., Coventry. OVE ARUP & PARTNERS INTERNATIONAL LTD. Structural Modelling Manual. Ove Arup & Partners International Ltd., London, 2002. DALLARD, PAT. Buckling – An Approach Based on Geometric Stiffness and Eigen Analysis. Ove Arup & Partners International Ltd., London, June 1998. MCKECHNIE, Steve. Buckling Analysis Using the Dallard Method in GSA. Ove Arup & Partners International Ltd., London, 2002. WILLFORD, Michael & YOUNG, Peter. Towards A Consistent Approach of Predicting Footfall-Induced Structural Vibrations. Advanced Technology Ove Arup & Partners International Ltd., London. FELTHAM, Ian. Berlin Floor Vibration Seminar 2003. Ove Arup and Partners International Ltd., London, 2003. WILFORD, Michael. An Investigation into Crowd-Induced Vertical Dynamic Loads Using Available Measurements. Ove Arup and Partners International Ltd., 2003. OVE ARUP & PARTNERS INTERNATIONAL LTD. Engineering for Structural Vibrations, Current Developments in Research and Practice. Ove Arup & Partners International Ltd., London, October 2001. OVE ARUP & PARTNERS INTERNATIONAL LTD. Dynamics and Buckling in GSA. Ove Arup & Partners International Ltd., London, 1999. DALLARD, FITZPATRICK, FLINT, LE BOURVA, LOW, RIDSDILL SMITH, WILLFORD. The London Millennium Footbridge. The Structural Engineer Journal Volume 79 / No. 22, Institution of Structural Engineers, London, November 2001. FELTHAM, Ian. Calculating the Shear Stiffness of Trusses and Frames. Structures Notes 2003NST_5b, Ove Arup & Partners Ltd., London, 2003. OVE ARUP & PARTNERS INTERNATIONAL LTD. Constrained Layer Bithuthene Damping Analysis with MSC.NASTRAN. Advanced Technology Group, London, 2000. POWELL, Daniel. Tuned Slosh Dampers. Arup Research and Development, Ove Arup & Partners Ltd., London, 2003. OVE ARUP & PARTNERS INTERNATIONAL LTD. Nonlinear Analysis and Form-finding in GSA. Ove Arup & Partners International Ltd., London, December 2002. BANFI, Mike and FELTHAM, Ian. Stability of Structures. Ove Arup and Partners International Ltd., London, 2003. BANFI, Mike and FELTHAM, Ian. Preparing for the IStructE Part III Examinations. Ove Arup and Partners International Ltd., London, 2003. OVE ARUP & PARTNERS LTD. An Arup Introduction to Structural Dynamics. Ove Arup & Partners International Ltd., London. Structural Engineering 1352 Structural Engineering Analysis and Design Second Edition 97. 98. 99. 100. 101. 102. 103. 104. 105. 106. 107. 108. 109. 110. 111. 112. 113. 114. 115. 116. 117. 118. 119. 120. 121. 122. 123. 124. 125. 126. 127. 128. 129. 130. 131. 132. 133. INSTITUTION OF STRUCTURAL ENGINEERS. Stability of Buildings. Institution of Structural Engineers, London, 1998. OVE ARUP & PARTNERS INTERNATIONAL LTD. Scheme Design Guide. Ove Arup & Partners International Ltd., London, 1998. GOODCHILD, C.H. Economic Concete Frame Elements. Reinforced Concrete Council, Great Britain, 1997. TRADA. Eurocode 5 1995 Design Examples J – Joints. Timber Research and Development Association, United Kingdom, 1994. BRITISH STANDARDS INSTITUTION. Structural Use of Timber Part 3 Code of Practice for Trussed Rafter Roofs BS 5268-3: 1998. BSI, London. TRADA. Trussed Rafters. Timber Research and Development Association, United Kingdom, July 1991. TRADA. Bracing for Non-Domestic Timber Trussed Rafter Roofs. Timber Research and Development Association, United Kingdom, 1999. INSTITUTION OF STRUCTURAL ENGINEERS. IStructE Part III Exam CD. Institution of Structural Engineers, London. STEEL CONSTRUCTION INSTITUTE. Steel Designers’ Manual 5th and 6th Editions. Blackwell Science, London, 1994, 2003. BRITISH STANDARDS INSTITUTION. Steel Codes of Practice BS 5950-Part 1:2000. BSI, London. BRITISH STANDARDS INSTITUTION. Loading For Buildings BS 6399-1, BS 6399-2, BS 6399-3. BSI, London, 1996. BRITISH STANDARDS INSTITUTION. Concrete Codes of Practice BS 8110-Part 1:1997. BSI, London. BRITISH STANDARDS INSTITUTION. Steel Bridge Codes of Practice BS 5400-Part 3. BSI, London. BRITISH STANDARDS INSTITUTION. Concrete Bridge Codes of Practice BS 5400-Part 4. BSI, London. BRITISH STANDARDS INSTITUTION. Fatigue Resistant Design of Bridges. BS 5400-Part 10. BSI, London. BRITISH STANDARDS INSTITUTION. Fatigue Design and Assessment of Steel Structures BS 7608:1993. BSI, London. BRITISH STANDARDS INSTITUTION. Masonry Codes of Practice BS 5628. BSI, London. BRITISH STANDARDS INSTITUTION. Timber Codes of Practice BS 5268. BSI, London. EUROCODE 8. Design Provisions for the Earthquake Resistance of Structures. European Committee for Standardization, Brussels, 1998. FEMA 356. Prestandard and Commentary for the Seismic Rehabilitation of Buildings. American Society of Civil Engineers. TRAHAIR. The Behaviour and Design of Steel Structures to BS 5950. BIRKHAUSER. Steel Construction Manual. MACGINLEY. Steel Structures Practical Design Studies. DENNIS LAM. Structural Steelwork Third Edition. TREVOR DRAYCOTT. Structural Element Design Manual. Great Britain, 1990. STEEL CONSTRUCTION INSTITUTE. Steelwork Design Guide to BS5950. Great Britain. STEEL CONSTRUCTION INSTITUTE. Handbook of Structural Steelwork. Great Britain. INSTITUTION OF STRUCTURAL ENGINEERS. Manual For The Design Of Steelwork Building Structures To BS 5950. Great Britain. INSTITUTION OF STRUCTURAL ENGINEERS. Manual For The Design Of Steelwork Building Structures To EC3. Great Britain. STEEL CONSTRUCTION INSTITUTE. Portal Frame Design in Europe Part 1 and Part 2. Great Britain. STEEL CONSTRUCTION INSTITUTE. Design of Structural Steelwork Lattice Framed Industrial Steelwork. Great Britain. SIRIA. Technical Note 068 Design for Web Openings. Great Britain. STEEL CONSTRUCTION INSTITUTE. Simple Connections. Great Britain. STEEL CONSTRUCTION INSTITUTE. Moment Connections. Great Britain. STEEL CONSTRUCTION INSTITUTE. Composite Connections. Great Britain. STEEL CONSTRUCTION INSTITUTE. Steel Detailers Manual 2nd Edition. Great Britain. STEEL CONSTRUCTION INSTITUTE. Wind Moment Design Of Low Rise Frames. Great Britain. 1353 Structural Engineering Analysis and Design Second Edition 134. STEEL CONSTRUCTION INSTITUTE. Wind Moment Design Of Unbraced Composite Frames. Great Britain. 135. BRE, SCI AND OVE ARUP. Worked Examples for the Design of Steel Structures. Great Britain. 136. BRE. Wind Digest 436 Part 1, Part 2 and Part 3. Great Britain. 137. MOSLEY. Reinforced Concrete Design Fifth Edition. Great Britain, 1999. 138. CHUDLEY. Construction Technology. Great Britain. 139. CHUDLEY. Advanced Construction Technology. Great Britain. 140. Birkhauser. Concrete Construction Manual. 141. EUGENE J. O’BRIEN. Reinforced and Prestressed Concrete Design. Great Britain. 142. ROBIN WHITTLE. Arup Reinforced Concrete Detailing Manual. Ove Arup, Great Britain. 143. CIRIA. Design and Construction of Joints in Concrete Structures. Great Britain. 144. INSTITUTION OF STRUCTURAL ENGINEERS. Design Recommendations for Multi-storey and Underground Car Parks. Great Britain, June 2002. 145. INSTITUTION OF STRUCTURAL ENGINEERS. Manual For The Design Of Reinforced Concrete Building Structures To BS 8110 2nd Edition. Great Britain. 146. INSTITUTION OF STRUCTURAL ENGINEERS. Manual For The Design Of Reinforced Concrete Building Structures To Eurocode 2. Great Britain. 147. INSTITUTION OF STRUCTURAL ENGINEERS. Standard Method of Detailing Structural Concrete. Great Britain, August 1999. 148. CIRIA. The Design of Deep Beams in Reinforced Concrete Guide. Ove Arup and Partners. Great Britain. 149. BCA and OVE ARUP. Worked Examples for the Design of Concrete Buildings EC2. Great Britain, 1994. 150. BIRKHAUSER. Timber Construction Manual. 151. CHING. Building Construction Illustrated. 152. STEP. Timber Engineering Step Lectures.Netherlands. 153. CHUDLEY and GREENO. Building Construction Handbook Fourth Edition. Great Britain, 2002. 154. OZELTON. Timber Designers Manual Third Edition.Great Britain. 155. TRADA. Timber Frame Construction (2001). Great Britain, 2001. 156. INSTITUTION OF STRUCTURAL ENGINEERS. Design of Plain Masonry in Building Structures. Great Britain. 157. CURTIN. Reinforced Masonry Designers Manual. Blackwell Science, Great Britain, 1995. 158. TOMLINSON. Foundation Design and Construction.Great Britain. 159. SUTTON. Solving Problems in Soil Mechanics. Great Britain. 160. CURTIN. Structural Foundation Designers Manual. Blackwell Science, Great Britain. 161. BCA. Design of Basement with Waterproofing.Great Britain. 162. COUNCIL ON TALL BUILDINGS AND URBAN HABITAT. Structural Systems For Tall Buildings. McGraw-Hill International, Singapore, 1995. 163. COUNCIL ON TALL BUILDINGS AND URBAN HABITAT. Tall Buildings: 2000 and Beyond. 164. BUNGALE S. TARANATH. Steel, Concrete, and Composite Design of Tall Buildings Second Edition. McGraw-Hill, United States of America, 1998. 165. MICHAEL CHEW YIT LIN. Construction Technology for Tall Buildings. 166. WOLFGANG SCHUELLER. Vertical Building Structure. New York, 1990. 167. STAFFORD-SMITH. Tall Building Structures: Analysis and Design. 1354

Structural Engineering Analysi

Recommend Documents